Pro/ENGINEER Fundamentals - Frequently Asked Questions

Thirty one (31) characters can be used in Pro/ENGINEER object names. This number does not include the extension, i.e., .prt, .asm, .drw, or the object version number, i.e., .1, .2, .3.

*Can upper case characters be used in Pro/ENGINEER object names?

Upper case characters cannot be specified in Pro/ENGINEER object file names. Upper case characters can be specified during object creation, however, the file will be written to disk using lower case characters only.

Config.pro

*What is the reason for using a config.pro file?

The config.pro file is used to control the environment in which Pro/ENGINEER runs. There are over 150 available options which allow control of a variety of different aspects, ranging from model display to default units to search paths used to retrieve assembly components. A full list of all available options can be found in Appendix D of the Fundamentals Guide.

*Is a default config.pro file created when Pro/ENGINEER is installed?

When Pro/ENGINEER is initially installed, there is no default config.pro file that is created automatically. However, a large number of the options do have default values which are used unless the option setting is changed in a config.pro file. Appendix D in the Fundametals Guide lists all of the default config.pro values in italics. There are two methods that can be used to create a config.pro file. The first method is to utilize any text editor, vi for example, and manually create the file. Each option should have its own line in the file, with the format being {Option Value}. The second method is to use the Pro/TABLE editor from within Pro/ENGINEER. Select Misc, Edit Config, then enter the name of the configuration file. At this point, a Pro/TABLE editor will be launched and you can enter in the appropriate information. When you exit the Pro/TABLE, the config.pro file will be written to your local directory.

*Where does Pro/ENGINEER look for config.pro files?

Pro/ENGINEER looks for config.pro files in 3 different directories in the following order:

1)loadpoint/text: Config.pro files residing in loadpoint/text will be read first.
2)The user's home directory: With UNIX systems, Pro/ENGINEER will read config.pro in the user's home directory. This is most commonly used for specifying user customized config.pro options such as colors and mapkeys.
3)Working directory: The directory in which Pro/ENGINEER is executed from is searched for a config.pro file.

If the same option appears in more than one config.pro file, the one that was read last will be utilized by the system.

*After config.pro is edited, why aren't the changes reflected?

After config.pro is edited, Misc, Load Config must be selected in order for the modifications to be reflected in the Pro/ENGINEER session, or Pro/ENGINEER can be restarted. Be aware that some config.pro options require Pro/ENGINEER to be restarted in order for config.pro modifications to be reflected.

*After config.pro is edited, is it necessary to restart Pro/ENGINEER?

After config.pro is edited, Misc, Load Config must be selected in order for the modifications to be reflected in the Pro/ENGINEER session, or Pro/ENGINEER can be restarted. Modifications to the following config.pro options require Pro/ENGINEER to be restarted:

graphics
edge_display_quality
cascading_menus
header_menu
header_menu_alignment
menu_item_font
menu_horizontal_hint
set_menu_width
system_background_color
system_curves_color
system_dimmed_menu_color
system_edge_high_color
system_geometry_color
system_hidden_color
system_highlight_color
system_letter_color
system_section_color
system_sheetmetal_color
system_volume_color
windows_scale

*What is the difference between config.pro and config.sup?

There are two main differences between config.pro and config.sup.

Unlike config.pro, config.sup can only be located in the loadpoint/text directory.

Config.sup options cannot be overridden by options found in any config.pro. Also, items contained in the config.sup can only have one entry per option. Keeping this in mind, it is important that items which can have multiple entries, such as "mapkey" and "search_path", are not specified in config.sup.

*Is there a limitation on the number of characters that can be included in a config.pro entry?

Each line in config.pro is limited to 80 characters. Environment variables can be used to specify config.pro values containing more than 80 characters. Refer to Appendix D of the Pro/ENGINEER Fundamentals Guide for details.

Managing Pro/ENGINEER files using DBMS

General:

*Where are Pro/ENGINEER objects stored when Dbms, Save is selected?

By default, Pro/ENGINEER objects will be stored to the current working directory.

If the working directory is changed using Misc, Change Dir, Pro/ENGINEER objects will be saved to the new directory.

If a Pro/ENGINEER object is retrieved from a directory other than the current working directory, Pro/ENGINEER will save the object back to the directory from which it was retrieved. If the user does not have write permission in that directory, the object will not be saved unless the config.pro option "save_object_in_current" is set to yes .

*What does Dbms, Save As do?

DBMS - Save As will make a copy of a specified Pro/ENGINEER object using a new name. Pro/ENGINEER initially prompts for the object that is to be copied; the current object being the default. At the second prompt, a new file name can be specified. Pro/ENGINEER will create this object in the current working directory.

*What does Dbms, Backup do?

DBMS, Backup can be used to save Pro/ENGINEER objects to a specified directory. The object will be saved in the specified directory using the original filename.

DBMS, Backup in Assembly, Drawing, or Manufacturing modes will save all related objects to the specified directory.

*What does Dbms, Rename do?

DBMS, Rename is used to change the name of Pro/ENGINEER objects in memory and on disk. Pro/ENGINEER will rename all versions of the object being renamed.

When renaming an object that was retrieved from directory other than the current working directory, the renamed object will be saved in the directory that the object was retrieved from.

*What does Dbms, Erase do?

Dbms, Erase is used to clear the specified object from workstation memory. This functionality will not remove objects from disk. Objects referenced by an active assembly or drawing can not be erased.

The ERASE OBJECT menu will appear with the following options:

	Current Only   Erase only the current object from memory.

        All            Erase the current object and all associated objects 
                       from memory.

	Select         Erase the current object and other selected objects.

*What does Dbms, EraseNotDisplay do?

Dbms, EraseNotDisplay is used to erase all objects from the current session,except for those that are currently displayed and any objects referenced by the displayed objects.

For example, if an assembly instance is being displayed at the time EraseNotDisplay is selected, the instance, the instance's generic, and it's components will not be erased.

There is a configpro option related to Dbms, EraseNotDisplay called "prompt_on_erasenotdisp".

yes (default) - a message window for each eligible object in question appears, asking if you want to first save the object before it is erased.

no - the system will immediately erase all eligible objects.

*What does Dbms, InstDbms do?

Dbms, InstDbms will save a particular instance of a part or assembly in a seperate file called an " instance accelerator file" (suffix ".xpr" for a part, ".xas" for an assembly). This file is used to retrieve particular instances quickly from disk rather than having to first retrieve the generic into memory, selecting the particular instance according to the family table, and then regenerating. Therefor, with this functionality the amount of time that it takes to retrieve an instance of a part or assembly from disk can be cosiderably reduced. The trade off is that more disk space will be used to store the accelerator files.

When Dbms, InstDbms is selected the INST DBMS menu appears with the following options :

	Inst Index	- create or update the Instance Index file for a specified directory 
	Update Accel	- create or update accelerator files for all instances currently in session
	Purge Accel	- examine each instance accelerator file and delete it if it is not 
			  current with the generic
	SaveAccelEnv	- brings up the SV INST ACC menu

When SaveAccelEnv is selected the SV INST ACC menu appears with the following options:

	none  (default)	- the system does not save the instance in a file seperate from the model.
	always 		- the system always saves the instance in a separate file
	explicit	- the system saves the instance in a separate file only 
			  when the instance is explicitly saved.

The config.pro option "save_instance_accelerator" can also be used to control instance accelerator files. The values for this config.pro option are also none(default), always, explicit. When you bring up the SV INST ACC menu, one of the options will be highlighted to reflect the last setting. That setting could have been either loaded from a configuration file or selected previously from this menu.

*Does Pro/ENGINEER overwrite existing objects when saving to disk?

Pro/ENGINEER will not overwrite existing objects while saving to disk. Objects are saved to disk with an object version number after the file extension. Pro/ENGINEER will create a new object file each time the object is saved, monotonically increasing the version number each time.

Example: A part called valve.prt will be initially written to disk as valve.prt.1. Subsequent storage of this object will result in the files valve.prt.2. valve.prt.3, etc. When an object is retrieved and the directory contains multiple versions of the same object, the object with the highest version number will be retrieved.

*What does the object version number indicate?

The object version number indicates the number of times the object has been stored. Objects are saved to disk with an object version number after the file extension. Pro/ENGINEER will create a new object file each time the object is saved, monotonically increasing the version number each time.

Example: A part called valve.prt will be initially written to disk as valve.prt.1. Subsequent storage of this object will result in the files valve.prt.2. valve.prt.3, etc. If the directory is purged, the object with the highest version will remain.

*Does Pro/ENGINEER offer an auto-save function?

Auto-save functionality is not currently implemented in Pro/ENGINEER. The "prompt_on_exit" config.pro option can be utilized to prompt the user to save objects in session before exiting Pro/ENGINEER.

*What happens if I run out of disk space while saving my objects?

If available disk space is depleted during storage, Pro/ENGINEER will issue the message:

	"object_name could not be saved: Check disk space or
	write access.  Error in storage. Check previous message (then
	press Enter):"

Pro/ENGINEER will not save any portion of the object to disk. Disk space must be made available before the object can be saved.

*What is the difference between Dbms, Erase and Dbms, Delete All?

Dbms, Erase removes the object from workstation memory. The object is not removed from disk.

Dbms, Delete All removes all versions of the object and all associated objects from disk. It is recommended to approach this menu selection with a great deal of caution. Creating backup copies of Pro/ENGINEER objects is considered good practice and can reduce the effect of accidental removal of data.

*Why is the following message given: "Check disk space and write access"?

The message "Check disk space and write access" is given if the amount of disk space required to save the object exceeds available disk space or if the user does not have write access to the specified directory.

*Why is the following message given: "PDM database object must be renamed by Pro/PDM application"?

By default, Pro/ENGINEER will not allow Pro/PDM objects to be renamed within Pro/ENGINEER. The config.pro option "let_proe_rename_pdm_objects" set to "yes" will allow Pro/ENGINEER to rename Pro/PDM objects.

Warning: Objects renamed in Pro/ENGINEER will be considered new Pro/PDM objects when submitted back to a Pro/PDM database.

Part Mode:

*Why aren't part files saved when Dbms, Save is selected in Sketcher?

While in Sketcher, the Dbms, Save functionality will save the section to disk rather than the part file. This functionality allows sections to be stored to disk for future use in feature creation. Section files are saved to disk with a .sec file extension. Once Sketcher is exited by either completing the feature creation or quitting, Dbms, Save will save the part file to disk.

*How are family table instances stored to disk?

All family table instance information is stored within the generic model. Pro/ENGINEER does not save a unique object file to disk for each instance.

*How can copies of a part be created?

The Dbms, Save As functionality allows copies of part files to be created using the following technique:

Select Dbms, Save As. Pro/ENGINEER will prompt for the name of the object to copy. The current object in memory will be the default. Pro/ENGINEER will then prompt for the name of the new object.

Assembly Mode:

*Does Pro/ENGINEER save all components each time an assembly is saved?

By default, Pro/ENGINEER does not store all assembly components to disk upon each Dbms, Save operation. Instead, Pro/ENGINEER will save the assembly file and only components that have been modified. By setting the config.pro option "save_objects", this can be changed. By using this option, Pro/ENGINEER can be instructed to save all dependent objects, save only the objects that were modified, or save modified objects and objects specified by the user.

*Where does Pro/ENGINEER save part files that are assembled from a directory different than the current working directory ?

By default, Pro/ENGINEER will store objects that are assembled from other directories back to the directory of origin. If the user does not have write access to the directory, Pro/ENGINEER will not store the objects in the current working directory, unless specific confi.pro options have been set. The config.pro options "override_store_back" and "save_object_in_current" allow greater control over this type of situation.

*What happens during storage of an assembly if its dependent part files are located in a write-protected directory?

By default, Pro/ENGINEER will only store modified objects and will always store objects back to the directory from which they were retrieved. Therefore, if a part from a write protected directory has been modified and Dbms, Save is selected, Pro/ENGINEER will not be able to save the object unless the config.pro options "override_store_back" and "save_object_in_current" are utilized.

*Why can't an assembly be retrieved after clearing it from memory or after starting a new session of Pro/ENGINEER?

During assembly creation, it is possible to add components to the assembly that are located in directories other than the current working directory. When the assembly is saved, the assembly file is saved to the current working directory while modified components are saved back to the directories of origin. If the assembly is cleared from workstation memory by either exiting Pro/ENGINEER or by selecting Dbms, Erase, All, and then retrieved, it is possible that Pro/ENGINEER will not be able to locate certain components. The config.pro option "search_path" can be used to specify directories which Pro/ENGINEER will search for objects. The config.pro file must contain a separate "search_path" option for each directory to be searched.

Refer to Appendix D of the Pro/ENGINEER Fundamentals Guide for details.

*How does Dbms, Save As function in Assembly mode?

In Assembly mode, the Dbms, Save As functionality allows any or all members of the assembly to be copied.

By default, after selecting Dbms, Save As, Pro/ENGINEER will prompt for the assembly to be copied and the new assembly name. A check mark can then be placed next to each assembly component to be copied or ALL_ASSEMBLY_NAME can be selected to copy all assembly components.

If a check mark is placed next to any of the components or if ALL_ASSEMBLY_NAME is selected, Pro/TABLE will be displayed where new component names can be specified in the cell adjacent to the original.

If Done is selected without selecting a component or ALL_ASSEMBLY_NAME, Pro/ENGINEER will create only a copy of the assembly which references the original components.

The config.pro option "model_rename_template" is used to create a user defined renaming scheme.

Refer to Appendix D of the Pro/ENGINEER Fundamentals Guide for details.

*Why do parts intersected by assembly features require renaming before they can be stored?

Assembly features which intersect assembly components alter the geometrical intent of the original object. When the assembly is in session, the component exists in memory in two different states. When Pro/ENGINEER tries to save the assembly, it is unclear which state of the component is to be saved. Pro/ENGINEER will prompt the user to save the object with a new name. This will create a copy of the object containing the geometric result of the assembly feature.

*What does the config.pro option "override_store_back" do?

If the config.pro option "override_store_back" is set to "yes", Pro/ENGINEER will save objects retrieved from other directories to the current working directory;

If "override_store_back" is set to "no", which is the default, objects will be saved in the directory of origin. If the option is set to "no" and the user does not have write access to the directory of origin, Pro/ENGINEER utilizes the config.pro option "save_object_in_current".

*What does the config.pro option "save_object_in_current" do?

When the config.pro option "save_object_in_current" is set to "yes", Pro/ENGINEER will save objects to the current working directory if the user does not have write access to the directory from which the object was originally retrieved. If the option is set to "no", Pro/ENGINEER will not save the object at all. This option should be used in conjunction with the config.pro option "override_store_back".

*What is the preferred method to make a copy of an assembly?

The Dbms, Save As functionality if the best way of copying assemblies.

*What is the preferred method to rename assembly components?

The following procedure should be used to rename assembly components:

Retrieve the assembly which contains the components to be renamed
In a sub-window retrieve the component to be renamed
With the component active, select Dbms, Save As and enter the new component name
Select Change Window and pick in the window containing the assembly
Regenerate the assembly
Select Dbms, Save to save the assembly which contains a reference to the new component name.

Drawing Mode:

*What is the preferred method to rename a drawing?

The Dbms, Rename functionality should be utilized to rename a drawing.

*What is the preferred method to copy a drawing and its model?

The following procedure should be used to create a copy of a Pro/ENGINEER drawing:

Select Dbms, Save As
Enter the name of the drawing to copy, or enter <CR> for the current drawing
Enter the new drawing name

The following procedure can be used to create a copy of a drawing and a copy of the drawing model:

Create a new directory
Select Dbms, Backup and specify the new directory as the destination. Pro/ENGINEER will create a copy the drawing and the model
Select Dbms, Erase and clear the current drawing from memory
Select Misc, Change Dir select the new directory as the current working directory
Retrieve the backup drawing
Select Mode, Part and retrieve the part to be copied in a sub-window
With the part active, select Dbms, Rename and rename the part
Select Change Window and pick in the window containing the drawing
Regenerate and save the drawing.

View Functions

General:

*How can the orientation of the default view be changed?

The default model orientation can be redefined by setting the config.pro options "x_angle" and "y_angle" to the desired values of the rotation, in degrees, of the object about the x and y axis. In addition, the model can be saved in user defined orientations by selecting View, Names, Save, and entering a unique view name. The model can easily be reoriented into the saved view orientation by selecting View, Names, Retrieve, and selecting the saved view name.

*How must Pro/ENGINEER be configured to recognize a spaceball?

No configuration is required within Pro/ENGINEER in order for a spaceball to be recognized. If Pro/ENGINEER does not respond to the spaceball, we recommend contacting your systems administrator or hardware vendor for diagnostics.

Shading:

*How can the quality of a shaded model be increased?

The quality of the shaded model can be increased be selecting View, Cosmetic, Shade, Quality. Specify the shade quality between 1 and 10; the number 3 is the default. Increasing the shade quality to higher values may result in an increase in shading time.

*When a shaded model is spun, why does it revert back to wireframe?

Pro/ENGINEER shaded models will revert to wireframe if the machine is not configured for hardware shading capabilities. In order to have the model remain shaded during a spin operation, the workstation must have an appropriate graphics card installed, and the "graphics" option in the config.pro file must be set based on the type of workstation being used. Refer to the Hardware Configuration Notes for specific details.

*How can a postscript file of a shaded model be created?

To create an encapsulated postscript (EPS) file of a shaded model select View, Cosmetic, Shade, Display, Postscript, and select one of the four supported EPS plotters. Select Output to PS to create the postscript file, or select Resolution or Image Size for additional options.

Refer to the Hardware Configuration Notes for details on EPS plotter support.

*Why aren't surface features displayed when the model is shaded?

When the config.pro option "shade_surface_feat" is set to "no", surface features will not be displayed when the model is shaded.

Colors:

*How is a color map be stored to disk?

A user defined color map can be stored to disk by selecting View, Cosmetic, Colors, Store Map. Pro/ENGINEER will create a file called color.map in the current working directory.

*Where does the color.map file need to be located in order for Pro/ENGINEER to recognize it?

The color map file, color.map, will be automatically loaded if it is located in the directory that Pro/ENGINEER is executed from.

*How many different colors can be defined and stored to the color.map file?

The exact number of colors that can be defined will vary, depending on the type of workstation and the graphics card that is being used. Higher end graphics cards will typically allow a greater number of colors to be defined.

*Why is the Transparency menu selection not available?

The transparency functionality is offered only only with hardware graphics configurations. Refer to the Hardware Configuration Notes for other items available with hardware graphics configurations.

On machines configured to use hardware graphics, the transparency functionality must be enabled by selecting View, Cosmetic, Colors, Transparency, Enable.

*When a color is assigned to a part in Assembly mode, why is the color not reflected in Part mode?

Colors assigned to parts in Assembly mode do not effect Part mode. This functionality allows assembly colors to represent a production operation done after assembling the individual parts, e.g., the application of paint.

*In Assembly mode, why does the part display with a different color than what was defined in Part mode?

Colors applied to components in Assembly mode will override colors defined at the Part level. To unset an assembly color, retrieve the assembly and select View, Cosmetic, Colors, Unset, Subassembly, and select the component in question.

Exploded Views:

*Why does a subassembly explode when the top-level assembly is exploded?

By default, subassemblies explode when the top-level assembly is exploded. The top-level assembly can be modified to specify which subassemblies and which parts within the subassembly to explode by selecting Modify, Mod Expld, Explode Comp. Select Expand from the EXPLD COMP menu and pick the subassembly in the COMPONENT EDITOR. Select Toggle Expld from the EXPLD COMP menu and pick the components in the COMPONENT EDITOR that are not to be exploded (changing the value to N).

*How can exploded views show the axes of the explosion?

This functionality is not currently implemented in Pro/ENGINEER. However, datum axes can be created using one of several available methods. The type of datum axis to use will depend on the specific situation.

*How can an exploded view be saved to a named view?

Exploded views can be saved to a name by exploding the assembly, then selecting View, Names, Save. When an exploded view name is retrieved, the assembly can be unexploded using View, Cosmetic, Un-Explode.

The Misc Menu

*What is the Misc, Change Dir menu selection used for?

The Misc, Change Dir menu selection allows the Pro/ENGINEER working directory to be changed. After selecting Change Dir, Pro/ENGINEER prompts for the "NEW DIRECTORY NAME". A full or absolute path name can be specified, or a question mark (?) can be entered which will bring up the SELECT FILE menu which provides an interface to navigate through the directory tree.

*What is the Misc, System menu selection used for?

When Misc, System is selected, Pro/ENGINEER will execute a system shell. The current working directory for this shell is the Pro/ENGINEER working directory. The Pro/ENGINEER session will be suspended while the system window is active. Exiting out of the system window will allow the Pro/ENGINEER session to continue.

*Why do the Pro/ENGINEER windows become inaccessible after Misc, System is selected?

The Pro/ENGINEER session will be suspended while the system window is active. Exiting out of the system window will allow the Pro/ENGINEER session to continue.

*What is the Misc, List Options menu selection used for?

The Misc, List Options menu selection will open a Pro/ENGINEER information window and provide a list of all the installed Pro/ENGINEER optional modules specific to the Pro/ENGINEER serial number being used, e.g., Pro/INTERFACE, Pro/SURFACE, etc.

*What is the Misc, Product Info menu selection used for?

The Misc, Product Info menu selection will open a Pro/ENGINEER information window giving the active Pro/ENGINEER serial number as well as the Revision of Pro/ENGINEER, and the software manufacturing datecode. This information is specific to your site and used by Parametric Technology Customer Support as a means of determining your software configuration and licensing.

*In Release 17.0 of Pro/ENGINEER, what is the Misc, Support Info menu selection used for ?

Note: In Release 17.0 of Pro/ENGINEER, the Misc, Support Info menu selection has replaced the Misc, Product Info menu selection.

The Misc, Support Info menu selection will open a Pro/ENGINEER information window providing the following information:

Licensing Information - Software Version - Serial Number - Pro/ENGINEER loadpoint directory - License Configuration (Locked or Floating) - All included Pro/ENGINEER options

Machine Information - Hostname - Username - CPU id - Pro/ENGINEER machine type - OS name, release, and version - Pro/ENGINEER graphics type

Auxiliary Application Information

Parametric Technology Information - Important phone and fax numbers - WWW home page address - Internet e-mail address - customer support address

This information is specific to your site and used by Parametric Technology Customer Support as a means of determining your software configuration and licensing. This information is written to a support.inf file in the current working directory of Pro/ENGINEER.

*In Release 17.0 of Pro/ENGINEER, what is the Misc, Mapkey menu selection used for ?

The Misc, Mapkey menu selection is used to create a mapkey by recording a series of menu picks and assigning these picks to a keyboard key or keys. The created mapkey can be stored in the config.pro file for use in other sessions of Pro/ENGINEER or be specified to be used in the current session only.

When Misc, Mapkey is selected the Mapkey dialog box appears with the following options.

	Define	- start recording the steps to be included in the mapkey.
	Done 	- stop recording the macro.
	Cancel 	- cancel current mapkey definition.
	Close	- Close the Mapkey dialog window

Trail Files:

*What directory does Pro/ENGINEER create trail files in?

Each time Pro/ENGINEER is executed, a trail file is created called trail.txt.n; where n represents the file version number which monotonically increases with each new file. By default, Pro/ENGINEER trail files are written to the current working directory. The config.pro option "trail_dir" can be used to specify a directory to which the Pro/ENGINEER trail files are to be written.

*Why is Pro/ENGINEER unable to execute a trail file with the file name "trail.txt"?

Pro/ENGINEER does not allow trail files to be executed to have the file name "trail.txt". The file must be renamed since Pro/ENGINEER creates a new file "trail.txt" each time the software is executed. Trail files must be in the format filename.txt; where filename represents a string other than "trail".

*What would cause a trail file to go out of sequence?

There are a many possibilities that would lead to a trail file going out of sequence. Before executing the trail file, the Pro/ENGINEER environment must be exactly the same as it was during initial creation of the trail file. For example, if the trail file retrieves a part and makes modifications to it, the same version of the part must reside in the same location as it was found initially. In addition, the same config.pro options must be utilized. If, for example, the display of datum planes was modified, this could cause an out of sequence error. If a trail file does go out of sequence, the user will be notified of the line number that could not be executed. To troubleshoot this type of problem, copy the original trail file to a backup name, then edit the original trail file by removing all the lines after the one that caused the out of sequence error. Also remove five to seven lines before the point of failure. At this point, rerun the edited trail file, then manually walk through the menu picks by viewing the backup trail file. By doing this, it will be clear what is causing the problem.

*Is there a way to force the trail file to stop after each menu pick?

With the config.pro option "set_trail_single_step" set to "yes", a trail file will stop after each trail file step. Entering a carriage return will allow the trail file to proceed.

*Is there a way to force the trail file to pause after each menu pick?

The config.pro option "trail_delay" will force a trail file to pause for a specified number of seconds between trail file steps. The value to the "trail_delay" option is the delay period specified in seconds.

Screen Layout

*How can the size of the Pro/ENGINEER working window be controlled?

The default size of the Pro/ENGINEER working window can be controlled using the config.pro option "windows_scale". The window scaling factor is specified as the value to the "windows_scale" option ranging from 0.5 to 1.0. The default value for the "windows_scale" option is 1.0.

Pro/ENGINEER must be restarted in order for modifications to the value of "windows_scale" to appear.

*How can the fonts used in the Pro/ENGINEER menus be changed?

The config.pro option "menuitem_font" can be used to change the Pro/ENGINEER menu fonts.

On UNIX systems, the value of the "menuitem_font" option must be the name of a font available at the X-server running Pro/ENGINEER. The "xlsfonts" command can be used to list available system fonts. Example:

menuitem_font times_bold

On Windows NT systems, the "menuitem_font" format should be:

-face name-point_size-weight-italic

The face name is found in the Fonts dialogue box within the Windows NT Control Panel; spaces are acceptable. Example:

menuitem_font -times new roman-18-400-0

Pro/ENGINEER must be restarted in order for modifications to the value of "menuitem_font" to appear.

*How can the default location of the Pro/ENGINEER working window be changed?

Pro/ENGINEER does not currently allow the default location of the Pro/ENGINEER working window to be redefined, however the scale of the working window can be modified using the config.pro option "windows_scale".

*Is it possible to prevent the second column of menus from overlapping the Pro/ENGINEER working window?

With the config.pro option "menu_horizontal_hint" set to "right", Pro/ENGINEER will place the second column of menus to the right of the primary menus i.e. the ENVIRONMENT menu will appear to the right of the MAIN menu instead of overlapping the Pro/ENGINEER working window. Be aware that the working window may require a scaling factor using the config.pro option "windows_scale" to provide ample screen space for the secondary menus to be displayed.

Pro/ENGINEER must be restarted in order for modifications to the value of "menu_horizontal_hint" to appear.

*How can a separate icon be made of each individual working window rather than inconifying the entire Pro/ENGINEER session?

With the config.pro option "iconify_entire_pro" set to "no", individual working windows can be inconified. The default value for "iconify_entire_pro" is "yes".

Mapkeys

*What would cause a mapkey to not work properly when it is executed?

The mapkey functionality allows a series of Pro/ENGINEER menu selections and keyboard input to be executed by a keyboard command. If a mapkey will not execute properly, check the following:

If the mapkey was defined during a session of Pro/ENGINEER, verify that the config.pro file has been loaded into the Pro/ENGINEER session using Misc, Load Config.
Verify that the mapkey syntax has been specified correctly in config.pro.
Verify that the first menu selection defined in the mapkey is displayed in an active Pro/ENGINEER menu.
Verify that each Pro/ENGINEER menu selection that the mapkey is calling is not "greyed out". In other words, a mapkey will fail if a menu selection can not be interactively picked with the mouse pointer.
Verify that the definition of the mapkey in config.pro does not exceed 80 characters.

*Where is the mapkey functionality documented?

The mapkey functionality is documented in Chapter 10 of the Fundamentals Guide, under the heading KEYBOARD MACROS.

*How can keyboard input be included in a mapkey?

Pro/ENGINEER will allow keyboard input from a mapkey, but only certain input is allowed. Only single strings are acceptable. For example:

	MAPKEY pt #PART; #CREATE; top_housing;;

Please note that the end of this mapkey definition contains two semicolons which defines a (CR). For more information, refer to Chapter 10 of the Fundamentals Guide.

*Is there a limitation in the number of characters that can be included in a mapkey?

All lines in config.pro are limited to 80 characters. Mapkeys containing many characters may be nested together to define a single operation:

	MAPKEY  sh #view; #cosmetic; #shade; #display; 
	MAPKEY  eps  %sh; #postscript; #PhaserII PX; #output to ps;

This example has the first mapkey "sh" making the menu selections to shade the model. The second mapkey "eps" executes the first mapkey "sh", defined by %sh, and then creates a plot file. For more information refer to Chapter 10 of the Fundamentals Guide.

*How can a mapkey be defined to turn datums on and off?

The display of datum planes is a toggle function in Pro/ENGINEER. One mapkey is used to toggle the display:

	MAPKEY dtm #ENVIRONMENT; #Disp DtmPl

*Why are mapkeys not recognized in config.sup?

Only the first mapkey defined in config.sup will be recognized in Pro/ENGINEER, per the definition of config.sup.

*Can keyboard function keys be used in a mapkey?

Function keys may be used for mapkeys and should be defined as follows:

	MAPKEY $F2 #FEATURE, #CREATE, #DATUM, #POINT

The "$" sign tells Pro/ENGINEER that F2 is the function key "F2" and not the alpha-numeric characters "F" "2". For more information refer to Chapter 10 of the Fundamentals Guide.

*How can a mapkey call another mapkey?

A mapkey may execute another mapkey. This is called nesting mapkeys:

	MAPKEY  sh #view; #cosmetic; #shade; #display; 
	MAPKEY  eps  %sh; #postscript; #PhaserII PX; #output to ps;

*How can screen input be included in a mapkey?

Screen input can be entered during the execution of a mapkey by placing one semi-colon after a menu pick that requires input. If two semi-colons are placed sequentially, the default value will be accepted. For example, to create a mapkey that will automatically create a new part, with a user-defined name, consisting of a default set of datum planes, the following syntax would be used:

      MAPKEY np #Mode; #Part; #Create; #Feature; #Create; #Datum; #Plane; #Default;

In this case, the mapkey would pause and wait for the user to input the name of the model, then continue on to create the default datum planes.

*Can a mapkey prompt for a screen pick, then continue?

A mapkey may prompt for a screen pick, however it cannot continue once the selection has been made. An alternative technique is to define a second mapkey which will continue once the screen selection has been made.

Customizing menus using menu_def.pro

*Where is there detailed documentation on the menu_def.pro file?

Detailed documentation can be located in Chapter 10 of the Fundamentals Guide under the heading CUSTOMIZING MENUS.

*Where does Pro/ENGINEER look for menu_def.pro files?

Similar to config.pro, menu_def.pro file can reside in any of 3 directories.

*How can a menu selection be added to the ENTERPART menu?

The menudef.pro functionality can not be used to add a menu selection to the ENTERPART menu.

*How can a menu pick be removed from a menu?

Pro/ENGINEER menu selections may not be modified or removed.

*Why doesn't a menu_def.pro menu selection work when it is picked?

If the added menu selection aborts prematurely, check the following:

If the menudef.pro file was created within the Pro/ENGINEER session, Pro/ENGINEER must be restarted in order for the modification to be recognized.
Verify that the menu syntax has been specified correctly in menudef.pro.
Verify that the first menu selection defined in menu_def.pro is displayed in an active Pro/ENGINEER menu.
Verify that the each Pro/ENGINEER menu selection that added menu selection is calling is not "greyed out", in other words, an added menu selection will fail if a menu selection can not be interactively picked with the mouse pointer.
Verify that the definition of the menu selection in menudef.pro does not exceed 80 characters.

*How can a new menu selection be placed at the top of a menu?

All menudef.pro menu additions will be displayed in the bottom of the target menu.

*How can menu_def.pro be used to create a new menu?

A menu_def.pro will not allow a new menu to be created. Only new menu selections can be added to existing menus.

Family Tables

*How can the names of family table items (features, dimensions) be changed so that the names that appear in the column headings are more descriptive?

To change the name of a feature, select Set Up, Name, select the feature, then enter the new name for the feature. To modify dimensions, select Modify, Dim Cosmetics, Symbol, then enter in the symbol to replace the dimension symbol, "d#".

*Is there a limit to the number of rows and/or columns that can be included in a family table?

Initially, only a certain number of rows may be added due to the size of the buffer, but if the Pro/TABLE is exited, then re-entered, more entries can be made. The current limit is 256 columns and 512 rows. As an alternative technique, other text editors, such as vi or jot, can be used in place of Pro/TABLE.

*How can negative dimension values be entered in a family table?

In order to enter negative values, the dimension symbol must be preceded by a "$" sign when added to the family table.

*What does it mean to have nested instances?

Nested instances refer to instances created within other instances.

*What are .ptd and .idx files? Can they be deleted?

A .ptd file is a text file containing all the information found in the family table, including all instance names and their current values. This is not required for part retrieval and can be deleted. However, the .ptd file can be used to edit the family table outside of Pro/ENGINEER. If an instance is deleted by modifying the .ptd file, subsequent retrieval of the generic will ask the user if he or she wishes to clean up the family table, at which point any modifications made to the .ptd file will be reflected in the internal family table. In addition, as soon as the generic is stored, the internally stored family table will take precedence over the local .ptd file, if one exists in the current directory. When a generic part is retrieved in a directory where an external .ptd file resides, the external file will take precedence over the internally stored family table. The name of the ptd file will always have the same prefix as the name of the generic part. The .idx file is an instance index file and contains a list of all current instances within a directory. During object retrieval using Search/Retrieve, all instances will be listed in the menu structure if the .idx file is present in the current working directory. The default name of all instance index files will be {directory_name}.idx.

*What should be done if a regeneration failure is encountered during Verify?

If a regeneration failure is encountered during verification of one of the instances, retrieve the generic part and modify the dimensions of the generic to those of the instance that failed. At that point, the reason for the regeneration failure of the instance can be determined.

*How can the listing of all instances be prevented from appearing in the menus when retrieving an object using Search/Retr?

To prevent all instances from showing in the Pro/ENGINEER menu structure, delete the instance index file, or set "menu_show_instances" to "no" in config.pro.

*How can a part or assembly instance be added to a Pro/ENGINEER drawing as a drawing model?

To add an instance as a drawing model, the instance must be specified from the menus, either by using the .idx file or using the In Session selection.

*What happens to the generic and all other instances if features are created on a part or assembly instance?

When a feature is created on an instance, the new feature is automatically placed in the family table and will be suppressed in the generic and all other instances.

*In an assembly family table, how can components be replaced with other part instances from the same family table?

In order to replace assembly components using an assembly family table, enter the name of the part instance in the family table cell, instead of entering Y or N.

*How can part features and dimensions be controlled by an assembly family table?

To control part features and dimensions from an assembly family table:

Create a part instance with the desired values.
Add the component to the assembly family table.
Replace the generic part with the appropriate part instance.

Pro/PROGRAM

*Why does Pro/ENGINEER sometimes ask to select From Model or From File? What is the difference between the two selections?

The From File menu selection will be displayed only if the original Pro/PROGRAM has been modified and there is text file of the program residing in the current working directory. If From File is chosen, the editor will display the most recent listing of the program that resides on the local disk.

The From Model menu selection will extract the current listing associated with the object. Upon initial creation of a Pro/PROGRAM, the user will not see these two choices, as Pro/ENGINEER will use the default listing associated with the model. After modifying the model file, then storing it to disk, the user will be asked if he or she wishes to incorporate any changes. If the changes are successfully incorporated, the model will be update accordingly and the design file will be deleted, once again leaving only the default model listing.

*What is a .pls and/or a .als file? Can they be deleted?

The file extensions given to the Pro/PROGRAM listings are .pls (for part files) and .als (for assemblies).These files are created when the user exits from the text editor after making modifications to the program listing. These files are automatically deleted when the modifications have been incorporated into the model.

*How can all the current values for all of the parameters driven by the program be checked?

To display all the current settings of the parameters used in the Pro/PROGRAM, select Relations, Show Rel.

*What functionality does the Instantiate selection offer?

The Instantiate function will automatically create an entry into a family table using all the current values of the parameters driving the Pro/PROGRAM.

Relations

*How can negative values be used in relations?

Negative values can be used in relations by preceding the dimension symbol with a "$".

*When writing assembly relations, what does the first and second number represent (d#:#)?

When part dimension symbols are shown in assembly mode, they contain two numbers (d#:#). The first number is assigned from within the part and is the same number that will be seen if the symbol was viewed from Part mode. The second number is assigned from within Assembly mode and is the number that appears in the assembly coding table. Each part in the assembly is assigned a unique second number.

*What is a coding table?

A coding table is created when assembly relations are written. The coding table lists each component and lists the number (or index) that has been assigned to the component. This list can be seen at the beginning of the relations file.

*How can relations be specified in family table instances?

Relations must be applied to the generic model. If separate relations are needed for instances, a solution would be to copy the instance to a new name, thus breaking its dependence on the generic, then create the appropriate relations.

*How can dimensional tolerances be included in a relation?

Dimensional tolerances can be included in a relation. As is the case with nominal dimension values, the dimension symbol must be used to write the relation. For dimensional tolerances, the symbols tp# and tm# are utilized.

*When should sketcher relations be used instead of part relations?

Sketcher relations should be used when the section of a feature will be changing at different locations. For example, when creating a variable section sweep, sketcher relations should be used.

*What would cause Add to be greyed out in the RELATIONS menu?

The Add menu selection in the RELATIONS menu when attempting to add a relation to a family table instance. Relations must be added to instances in the generic model.

*Are relations stored separately from the part file?

All relations are stored within the part or assembly file.

*How can the default relations editor be specified?

The editor used to edit the relations file can be specified using the config.pro option "relation_file_editor". The value of "relation_file_editor" should be the system command entered at the command line to execute the editor.

To use the "jot" editor on Silicon Graphics Systems with Irix 5.2, specify "jot -f" as the "relation_file_editor".

*What is the difference between Relations, Evaluate and Datum, Evaluate?

When Relations, Evaluate is selected, Pro/ENGINEER prompts for a dimension symbol i.e. d4 d9, and returns the current value of that dimension. The Feature, Create, Datum, Evaluate function creates an "Evaluate feature" that will capture a measurement on the model and utilize that value in other relations.

*While writing a relation, a message appears that says, "Cannot assign to a part driven value." Why?

Dimensions that are already being driven by a relation at the part level cannot be directly driven by an assembly relation. Try adding a relation that drives the dimension in the part that is driving the actual dimension that you want to affect. For example, if you had a part relation of "d4=d2," and you also wanted "d4" to equal an assembly dimension, write the relation so that "d2" is driven, as in "d2:8 = d5:0." This relation would also cause "d4" to equal "d5:0." This example assumes that the coding symbol for the part is "8," and the coding symbol for the assembly is "0."

Layers

*What are layers used for?

Layers are used to group items together to allow various operations to be performed on the items as a group, as opposed to performing these operations on individual items. One of the most common uses for layers is to blank or display sets of non-geometry features, such as datum curves or datum planes, which were used to construct a model, but are not needed in the display of the final product. Other uses include the suppression of multiple features at one time and greater control over assembly display by blanking and/or displaying assembly components.

*What types of items can be placed on a layer?

In part mode, any type of feature can be placed on a layer. However, only non-geometry items, such as datum curves or surface features, can have their display manipulated. If a geometry feature, such as a hole or a protrusion, is added to a layer, and that layer is blanked, the item will still appear. However, groups of geometry features can be suppressed by layers.

In assembly mode, individual components or sub assemblies can be placed on a layer and can have their display status changed by either selecting display or blank. Assembly features can also be added to layers, but, as is the case in part mode, only features that do not physically alter the geometry can be blanked and displayed.

In drawing mode, any 2D items, such as notes, symbols, or dimensions can be added to a layer. Drawing tables can also be placed on a layer.

*What is the difference between blanking and displaying a layer?

When a particular layer is blanked, any non-geometry item that has been placed on that layer will not be displayed. Conversely, when a layer is displayed, ONLY the items on that layer will be displayed. In part mode, any items that are on other layers will not be displayed. In assembly mode, all other items, including components that do not belong to any other layer, will not appear.

*Is it possible to blank features, such as cuts or protrusions?

Any feature that physically modifies the geometry can be added to a layer, but can not be blanked or displayed. Only non-geometry items can have their layer status changed. Groups of geometry features can be placed on a layer and that layer can be supressed.

*How can the current status of all layers be retained in order to have the same layer settings the next time the part is retrieved?

Pro/ENGINEER will not automatically save the current layer status when an object is saved. By default, the layer status for all layers will revert to normal each time the object is retrieved into session. If it is determined that the current layer status is to be used the next time the part or assembly is retrieved, the Save Status menu pick must be selected. This is found by selecting View, Layer Disp.

*In assembly mode, why can't certain components be placed on a layer?

If a component can not be selected for placement on a layer at the current assembly level, this indicates that the component is a member of a sub-assembly. Only that entire sub-assembly can be placed on a layer at the current assembly level. In order to place the component on a layer individually, the layer must be created at the sub-assembly level at which the component was placed.

Parent Child Relationships

*What is meant by a parent-child relationship?

When a feature is created in Pro/ENGINEER, dimensional and geometric references are created. These references, whether they are edges, surfaces, or vertices, will belong to other features that already exist on the model. When such a reference is established, this is referred to as a parent-child relation. The newly created feature is now considered a child of any feature that contains an entity that was used as a reference.

*How can a feature have more than one parent?

Yes, a feature can have more than one parent. For example, if a cut is created in such a way that the sketching plane chosen was a surface on the base feature and then the cross section of the cut has a dimension that defines a distance from a datum plane, both the datum plane and the base feature are considered parents of the cut.

*How can a feature have more than one child?

Yes, a feature can have more than one child. It is not uncommon for the first feature of a model to have dozens of children. For example, if a default set of datum planes is the first set of features created on a model, all subsequent geometry will be children of one or more of these datum planes. The initial feature will typically use two of the datum planes for references, one as a sketching plane and one as vertical or horizontal reference. In addition, any feature that uses this newly created feature as a reference will now become a child of the the datum planes that are the parents of the first feature.

*What will happen to a child if a parent is deleted or suppressed?

If a feature containing children is selected to be deleted or suppressed, Pro/ENGINEER will highlight the child in blue and ask for an action to be taken. Without the parent, the child will not have a complete set of references and will not be able to regenerate. Therefore, when attempting to delete or suppress a parent, the child must be rerouted, deleted (or suppressed), or suspended. These options will be listed in the CHILD menu, which will appear automatically when attempting to delete or suppress a feature with children.

*How can a list of all parents and/or children of a specific feature be obtained?

In order to obtain a complete list of parents or children of a particular feature, select Info, ParentChild. At that point, a prompt will appear asking if information on parents or children is desired. Once this selection is made, select the desired feature, and the information will be displayed.

Pro/TABLE

*How can Pro/TABLE be utilized without running Pro/ENGINEER?

Pro/TABLE is a stand-alone program that can be invoked without using Pro/ENGINEER. To execute a session of Pro/TABLE from a command line, type in the command "protab". This allows bend tables, family tables, and drawing setup files to be edited outside of Pro/ENGINEER.

*How can the width of the Pro/TABLE columns be modified?

The width of a Pro/TABLE column can be changed by selecting Format from the Pro/TABLE menu. All of the columns can be changed by selecting Global Width, or some of the columns can be changed by selecting Column Width and highlighting the desired cells. In order to reset the column width back to the default value, select Format, Reset Width.

*After using Pro/TABLE, why does system speed decrease?

After utilizing a session of Pro/TABLE, the size of the buffer used to write data to the trail file will increase. If the trail files are being written across an NFS mount, i.e., if the Pro/ENGINEER startup directory is a shared filesystem that has been mounted across the network, there may be a noticeable decrease in system speed. To solve this, set the config.pro option "trail_dir" to a directory that is local to the Pro/ENGINEER client machine.

Is there a limit on the number of rows and columns that can be used in a Pro/TABLE editor?

In post 14.0 releases of Pro/ENGINEER there is no limit as to the number of columns and rows that can be used in Pro/TABLE

In 14.0 and earlier releases of Pro/ENGINEER, the limit for the number of entries into Pro/TABLE is 256 columns and 512 rows. If more data needs to be entered, alternate editors, such as vi or jot, can be utilized.

*Where is there additional information documented regarding Pro/TABLE functionality?

Additional information regarding Pro/TABLE functionality can be located in Appendix C of the Fundamentals User Guide.

Frequently Asked Questions Pro/ENGINEER Fundamentals

Back to Technical Information on Pro/ENGINEER

Topics: I. Configuring Pro/ENGINEER Config.pro Screen Layout Mapkeys menu_def.pro Object Names II. Controlling Designs Relations Parent Child Relationships Family Tables Pro/PROGRAM Layers III. Main / View View Misc DBMS IV. Other Pro/TABLE

Pro/ENGINEER Object Names

Config.pro

Managing Pro/ENGINEER files using DBMS

View Functions

The Misc Menu

Screen Layout

Mapkeys - Keyboard Macros

Customizing Menus using menu_def.pro

Family Tables

Pro/PROGRAM

Relations

Layers

Parent Child Relationships

Pro/TABLE

Pro/ENGINEER Object Names

Config.pro

Managing Pro/ENGINEER files using DBMS

View Functions

The Misc Menu

Screen Layout

Mapkeys

Customizing menus using menu_def.pro

Family Tables

Pro/PROGRAM

Relations

Layers

Parent Child Relationships

Pro/TABLE

Topics:
I. Configuring Pro/ENGINEER

Config.pro
Screen Layout
Mapkeys
menu_def.pro
Object Names

II. Controlling Designs

Relations
Parent Child Relationships
Family Tables
Pro/PROGRAM
Layers

III. Main / View

View
Misc
DBMS

IV. Other

Pro/TABLE