Will Pro/ENGINEER convert a materials file into different units if the part units change?
What are the units in a materials file?
Where are material files written?
What does the config.pro option "pro_material_dir" do?
What does the message: "Error: Cannot find materials file" mean?
After changing the model units, why do datum planes display very large?
After changing the model units, why are some features not scaled?
Can parts of differing units be assembled?
How can the model units be displayed?
After modifying the model units, why would the values of the dimensions remain unchanged?
After modifying the model units, why would the values of the dimensions change?
How can the distance between two points be measured?
How can distances along a swept trajectory be measured?
How can the distance between a pipe and a component in pipe mode be measured?
How to find the closest point between two curves?
What is the FEATURE NUMBER refer to when Feat Info or Model Info is selected?
What is the INTERNAL FEATURE ID refer to when Feat Info or Model Info is selected?
What does an asterisk (*) indicate when Feat Info or Model Info is selected?
How can information be found on which layer contains which items?
If the BOM appears to be missing information, verify that the text lines do not wrap around to the next line in the BOM format file. Any information that continues to the next line will not appear in the BOM. Additionally, verify that the last line contains a carriage return.
*What should the BOM of a Simplified Representation contain?
Simplified Representions will still contain the full listing of all the components in the Master Simp Rep.
Pro/ENGINEER will not automatically convert material property file units if the part units are changed. Material files are numberic values that can be referenced as parameters on a Pro/ENGINEER drawing with the exception of Density. Different materials files (eg material_in.mat and material_mm.mat) can be created when needed as called out in the config.pro option "pro_material_dir".
*What are the units in a materials file?
Pro/ENGINEER material files have no units. The material files contain numeric values for properties to be referenced later i.e. on a Pro/ENGINEER drawing. Please note that the material file parameters are not used in mass property calculations with the exception of Density.
*Where are material files written?
By default, Pro/ENGINEER will write material files to the current working directory. The config.pro option "pro_material_dir" can be used to specify a directory in which the material files are located.
*What does the config.pro option "pro_material_dir" do?
This option allows Pro/ENGINEER to find user defined materials files on disk when assigning materials to parts. Note that Pro/ENGINEER will not automatically place the material.mat file from the current working directory to the materials file directory. The file must be placed there manually.
*"Error: Cannot find materials file." What does this mean?
This error is generated when Pro/ENGINEER is unable to locate the specified materials file in one or both of the following directories:
Imported geometry such as IGES features will not be modified when the model units are modified. The datum planes features stay with the default size of the part.
*Can parts of differing units be assembled?
Pro/ENGINEER assemblies can contain components consisting of different model units. The assembly also has its own units. Note: assembly features can not intersect a part that has different model units than the assembly. Pro/ENGINEER will prompt: "Can not select part with units different from that of the assembly."
*How can the model units be displayed?
The following techniques can be used to display model units:
Technique One:
Modification of model units using the Same Dims functionality will will force Pro/ENGINEER to change the model units while keeping the numeric value of the dimensions the same. Example: a dimension of 1.00 inches will be converted to 1.00 mm when the model units are changed from inches to millimeters.
The Same Size menu selection can be used to change the numeric value of the dimension when the model units are changed, keeping the geometry the same size. Example: a 1.00 inch dimension will be converted to 25.4mm when the model units are changed from inches to millimeters.
*After modifying the model units, why would the values of the dimensions change?
Modification of model units using the Same Size functionality will will force Pro/ENGINEER to change the numeric value of the dimension when the model units are changed, keeping the geometry the same size. Example: a 1.00 inch dimension will be converted to 25.4mm when the model units are changed from inches to millimeters.
The Same Dims menu selection can be used to change the model units while keeping the numeric value of the dimensions the same. Example: a dimension of 1.00 inches will be converted to 1.00 mm when the model units are changed from inches to millimeters.
To measure the shortest distance between points, select the desired points with Absolute selected in the DISTANCE menu. To display the X, Y, and Z distance between points, select Increment from the DISTANCE menu and select the appropriate Coordinate System from which to measure. Pro/ENGINEER will export dx, dy, and dz accordingly.
Creating datum planes that pass through the points in the direction to be measured can also be used to obtain the distance between points by measuring the distance between the plane and points.
*How can distances along a swept trajectory be measured?
To obtain the distance along a swept trajectory select Info, Measure, Curve/Edge, Length. The Datum Evaluate feature will also allow parameters to be assigned lengths of curves and edges to be used later i.e. in relations.
*How can the distance between a pipe and a component in Pipe mode be measured?
Distances can only be measured in assembly mode using Info, Measure and selecting the proper references.
*How to find the closest point between two curves?
In order to find the closest point between curves, create a datum point that is the closest point on the first curve to the second curve and vice versa. Once the location of these points is known, create a datum curve between the two. The midpoint, which can found using a datum point created on curve using an offset lenght ratio of 0.50, of the this new curve is the closest point between the two original datum curves.
*How to export the coordinates of datum points?
To find the coordinates of one datum point with respect to a coordinate system, use the Distance functionality in the INFO Measure menu. Perform a From Csys - To Point measurement using the INCREMENT option. The resulting information is the dx,dy and dz of the datum point which are equivalent to the x, y, z coordinates.
To export the coordinates of a large number of datum points to an a text file for use in another application, first export the whole model as an IGES file using the Dtm Curves option. In a new part with a default coordinate system, create datum points using the offset from csys method. Read the points from the IGES file by entering the name of the file with the .IGS extension. Pro/ENGINEER will then read all the points from the IGES file. Once the creation of the datum points has been successful, modify the datum points and pick Edit Table points to see the x, y, z coordinates in a three column format.
The FEATURE NUMBER is the sequential number that Pro/ENGINEER uses during regeneration. Pro/ENGINEER will always maintain the order starting from 1 until the last active (ie non-Suppressed) feature. The FEATURE NUMBER will change if features are Reordered, Suppressed, and/or Resumed.
*What is the INTERNAL FEATURE ID refer to when Feat Info or Model Info is selected?
The INTERNAL FEATURE ID is an internal number generated by Pro/ENGINEER for each feature. Each feature's INTERNAL FEATURE ID will not change when model features are suppressed, resumed, reordered, or deleted.
*What does an asterisk (*) indicate when Feat Info or Model Info is selected?
The asterisk (*) indicates the feature is currently in a suppressed state. The Feature, Resume selection can be used to "activate" the feature. Please note that information can be obtained while the feature is suppressed by selecting Info, Feat Info, Sel By Menu and specifying the feature's"INTERNAL FEATURE ID".
*How can I find which layer contains which items?
Select Info from the LAYER menu, or select Layer Info from the INFO menu to find a listing of all items associated with any given layer. Non-solid geometry (eg datum planes) will also list layers associated with that feature by picking Feat/Model info and picking the desired feature.
Send comments to webmaster@ptc.com
Copyright © 1995 Parametric Technology Corporation
,128 Technology Drive, Waltham, MA 02154. All rights reserved.