What is the best method to determine the orientation and view of each particular section?
How are lines, arcs, and circles created?
How is an arc length dimension created?
How is an angular dimension for an arc created?
How is a diameter dimension created?
How are multiple sketched entities aligned to existing geometry at once?
What informs the user that an entity is aligned?
Certain edges cannot be selected as a dimensioning or aligning reference, why?
Why is Unregenerate sometimes unavailable?
What is the difference between a local coordinate system and a datum coordinate system?
How can the orientation of a local coordinate system be changed so that the x-direction is vertical?
How is a conic created and dimensioned?
How is a spline created and dimensioned?
How can the points of a spline be moved?
How is a spline constrained to be tangent at the endpoints?
How can entities that have been removed with Delete be recovered?
How many deleted entities can be recovered through Undelete?
How does Pro/ENGINEER determine the size of a fillet created from the ARC TYPE menu?
How can the theoretical sharp corner of a fillet be determined?
Can a spline be aligned to existing geometry?
When are Sketcher relations evaluated?
Do entities created as Concentric need to be constrained through Dimension and/or Align?
What is an Ordinate dimension?
How are Sketcher assumptions avoided?
How is the number of decimal places modified in Sketcher?
What is trajpar and how is it used?
Why do all the verticies of a sketch highlight red when it is regenerated?
Do the highlighted "extra dimensions" found by regenerating a sketch have to be deleted?
How to sketch multiple sections for blend feature?
How may an arc be sketched such that it's endpoint is tangent to an existing model edge?
Will the Tangent End option work when attemptint to sketch an entity tangent to a spline?
Can a section from a previously created part be retrieved into Sketcher?
How can a sketcher assumption be disabled?
How can the radius of curvature for a spline be dimensioned?
Underdimensioned Section. Please align to part or add dimensions.
Regeneration completed successfully. EXTRA DIMENSIONS FOUND.
Locate section with respect to part.
Section must be closed for this feature.
Section must be open for this feature.
Warning: Not all open ends have been explicitly aligned.
References to additional 3-D geometry cannot be made.
Highlighted arc with conflicting constraints.
For open sections, the start points must be end points.
Must have more than one section. Select "Sec Tools", "Toggle" for next section.
Number of entities per section must be equal.
WARNING: This entity is referenced by other feature(s). Continue? [N]:
What side of the bounding entity should be selected when using Trim?
When Mirror is used, does Sketcher create new entities or extend the original?
What is the difference between Intersect and Trim?
What is the simplest method of trimming two entities to one another?
How can sketched entities be relocated without having to delete and recreate them?
How can a group of sketched entities be relocated without having to recreate and attach them?
How can solid geometry be copied into a feature's section?
Can the sketching references of a feature be changed once in Sketcher mode?
Can the Sketcher grid be changed?
How can the arc length of an entity be determined?
How does the accuracy of Sketcher mode differ from that of Part mode?
How are 2D IGES files imported into Sketcher?
Can 3D IGES data be imported to Sketcher?
Why are section entities underdimensioned if they were created as imported IGES data?
Are sections plotted with the Sketcher grid?
How can the direction of a start point be changed?
How can sections be retrieved into Sketcher mode?
What sub-section is active when nothing is highlighted in cyan after selecting Toggle?
Is it possible to import DXF files into Sketcher?
Is it possible to import TIFF files into Sketcher?
Pro/ENGINEER creates features in certain directions. Protrusions are created coming out of the screen at you, and cuts are created into the screen away from you. The arrow that appears upon selecting the sketching plane may define the direction of feature creation or the viewing direction, depending on the feature type being created. If the particular viewing direction of the section is not evident to the user, sketch an entity and then select View, Default. This will reset the model to a Trimetric or Isometric view, depending on the ENVIRONENT setting, and the sketched entity will appear in cyan. This should provide a clear understanding of the sketching orientation. Select Sketch in the sketcher menu to return to the sketching plane orientation.
Using Mouse Sketch, lines are created with the left mouse button, each click indicating an anchor point for the "rubberband" line. The line entity is finished by selecting the middle mouse button. Different types of lines can be created through the LINE TYPE menu, including Horizontal, Vertical, Parallel, Perpendicular, Tangent, and 2 Tangent. 2 Tangent lines are connected between two arcs, splines, or circles, and split the referenced entities.
While using Mouse Sketch, arcs can be created at the endpoint of sketched entities with the right mouse button. This arc will be tangent to the entity to which it is attached. If a line is being sketched, the middle mouse button must first be depressed to end the line, then the right button will activate a tangent arc. Other types of arcs are Fillet, Concentric, 3 Point, Ctr/Ends, and 3 Tangent. Any arc types selected from the ARC TYPE menu must be created with the left mouse button, middle button aborting the sketch.
Circles can be created with Mouse Sketch by selecting the middle mouse button to anchor the center point, and then again to determine the diameter. Other types of circles can be sketched using the CIRCLE TYPE menu, including Concentric, 3 Tangent, Fillet, and 3 Point. Any options selected from the CIRCLE TYPE menu must be created with the left mouse button, middle button aborting the sketch. Construction circles display in centerline format and act as references for sketched entities. Construction circles will not create geometry.
Arcs cannot be constrained with arc length dimensions. The valid dimension schemes include radii, linear, and angular. If an arc length scheme is necessary for driving a feature, use relations or evaluate features. The arc length of a segment can be determined in the SEC INFO menu.
An arc can be dimensioned with an angular constraint by first selecting each endpoint and then the arc itself, with the left mouse button, and then placing the dimension with the middle mouse button.
A diameter dimension is created by selecting a circle or arc twice with the left mouse button, then placed with the middle mouse button.
By selecting the model geometry with the left mouse button, and then depressing the middle button, all entities within the immediate proximity that can be aligned, will be aligned.
When the Align command is successful, Pro/ENGINEER will return a confirmation message "-- Aligned --". Alignment can be later investigated by selecting Unalign from the ALIGNMENT menu, and all aligned entities and their model references will highlight in green.
Silhouette edges of model geometry that are not in the plane of a sketch cannot be selected for reference through Align, Use Edge, Offset Edge, and Dimension.
Unregenerate is available immediately after regeneration is successful. It allows the user to revert back to the state prior to regeneration. The sketched geometry will be restored to what it was, and dimensions will retain their modified value. The dimensions will be displayed in white, defined as unregenerated values.
An Adv Geometry Coord Sys is referred to as a local coordinate system. It belongs to the section in which it is created, and will only be displayed in that sketch. These entities are used for dimensioning references, splines, and blend features.
By default, local coordinate systems are always placed with the x-axis horizontal and the y-axis vertical. These entities can be rotated and translated through Move. Rotate90 will spin the local coordinate system about the z-axis, which is always normal to the screen, in 90 degree increments.
A conic is created through Adv Geometry, Conic. This type of entity is created by selecting the endpoints and then the shoulder of the conic, all with the left mouse button. Conic endpoints are dimensioned for location and then for tangency. Tangency is created using angular dimensions at the endpoints. First select the conic, then the endpoint, then the entity being referenced, and finally depressing the middle mouse button to place the dimension. The shoulder of the conic also needs to be constrained. This is done in one of two ways, using a "rho" value, or a Sketcher point. The rho value is defined by selecting the conic and placing the dimension with the middle mouse button. The second technique creates a point through Sketch, Point to anchor the shoulder. This point needs to then be constrained through Dimension and/or Align. Refer to the Sketcher section of the Pro/ENGINEER Part Modeling User's Guide.
A spline is created through Adv Geometry, Spline. This type of entity is created by selecting points that the curve will smoothly pass through. The endpoints of a spline can be further defined with tangency and curvature to control the spline's shape. A spline can be dimensioned to a local coordinate system by selecting Dimension, selecting the spline once, then again, ensuring not to select one of the points, selecting the coordinate system, and finishing the dimension with the middle mouse button.
A spline must first be dimensioned to a local coordinate system for these options to be available.
Spline points can be modified in several methods, each method is accessed by first selecting Modify and selecting the spline. The individual points can be selected and dynamically dragged through Move Pnts. Point locations modified through Coords will allow the user to enter a numeric value for the x and y locations, with respect to the local coordinate system. Refer to Step #11 - Suggested Technique for Creating a Spring as a Base Feature. The entire array of spline points can be output to a text file and edited in a system editor. The locations are output using Save Pnts, and can then be edited outside of Pro/ENGINEER through a System window and brought back into the section with Read Pnts.
Tangency is established by first selecting Modify and selecting the spline, then choosing Tangency. Angular dimensions can be added to the spline endpoints by selecting the spline once, then again, ensuring not to select one of the points, the endpoint, the reference entity, and then the middle mouse button to place the dimension.
Entities removed with Delete can be recovered using Undelete, in the DELETION menu.
Sketcher will remember up to 10 entities that were deleted. After a Regenerate the Delete memory is cleared and any deleted entities can no longer be undeleted.
Pro/ENGINEER creates an entity through Arc, Fillet so that it passes through the selected entity location that is closest to the intersection point. If two lines forming a right angle are selected for a Fillet, the arc will pass through the point of selection that is closest to their intersection.
The theoretical sharp corner of a fillet can be determined by sketching a Point on the intersection of the entities before the fillet is created, or at the intersection of centerlines that pass through the edges.
Both endpoints and internal points of splines can be aligned to existing geometry. A spline itself cannot be aligned, but can be associated to a local coordinate system for shape definition.
Sketcher relations are evaluated when the section is regenerated. The section is regenerated when the user is creating, modifying, or redefining the feature.
The center points of arcs and circles created through Concentric are automatically aligned to the center point of the geometry that is referenced. Radius or diameter dimensions do need to be defined to entirely resolve the entity.
This type of dimension references only part geometry, not section entities. These dimensions are used to drive sketcher dimensions through relations, and are only displayed in the particular section where they are created.
Linear dimensions can be created in an Ordinate scheme by first creating the Baseline dimensions, then selecting the baseline dimension and the entity to be dimensioned. The dimension is placed with the middle mouse button.
Sketcher assumptions are best avoided by exaggerating the sketch. If two lines should not be the same size then they should not be sketched at about the same length. If an angle is going to be very small, sketch the entities at a large angle to one another and make the modification in Part mode to the required dimension.
The number of Sketcher decimal places can be set with the config.pro option "sketcher_dec_places", the default value being 2. This will ensure that every section that is created will have the same number of decimal places. If a number of decimal places other than the default is required, selecting Sec Tools, Set Up, Num Digits will change all of the dimension decimal places.
Evalgraph is a system parameter used for driving dimensions in Sketcher relations of swept features, according to a user-defined graph feature. The y-axis of the graph feature drives the dimension as the section travels along the trajectory represented by the x-axis. Evalgraph is used in conjunction with trajpar.
This indicates that the sketched section has not been located with respect to the existing geometry. Additional dimensioning is required between Sketcher entities and existing geometry and/or alignlment of Sketcher entities to existing geometry is necessary for the sketch to regenerate.
Sketcher will need to have enough dimensions to fully define the section. If additional dimensions are found, either the highlighted dimension(s) or alternate dimensions may be deleted. If entities have been aligned, they may be unaligned. If these "extra dimensions" are not deleted, they will remain as reference dimensions which cannot be modified but may be used in relations.
When a feature section is created, the dimensions of the sketched entities are proportional to the rest of the model. If default datum planes are created as the first feature in a part, the sketched entities will have dimensions proportional to the "size" of the default datums. In Sketcher, the default grid spacing for a model consisting only of default datum planes is 30.0000. If no features exist when the first section is sketched, the default grid spacing is 1.0000.
Sketch the first section and regenerate successfully. Then select Sec Tools, Toggle. The Section will now appear grey. Sketch the second section.Repeat this process as necessary to create the desired number of sections for the feature.
Use Geom Tools, Use Edge to copy the model edge the arc will be tangent to. Trim the entity to the point the arc will be tangent to. Sketch the arc using the Tangent End option. Then delete the original entity created with the Use Edge option as necessary.
No, when sketching an arc, the Tangent End option works only when the referenced entity is a line or an arc.
Retrieve the previously created part. Identify the feature which is defined by the desired section. Redefine that feature selecting Section and Sketch. when the sketch appears, Save the section using the Dbms options. Return to the new Sketcher window and procede to retrieve the section using Sec Tools, Place Section.
From the sketcher menu, select Constraints. The Constraint Display dialog box should appear. Select the constraint to be disabled, followed by Disable. Select OK to confirm the new constraint status information.
From the SKETCHER menu, select Dimension. With the left mouse button, select the endpoint of the spline and then place the dimension with the middle mouse button. The dimension will be shown with a leader off of the endpoint of the spline. For an example of dimensioning the radius of curvature, please refer to the Suggested Technique for Dimensioning the Radius of Curvature of a Spline
If there is not enough information to solve the section, Pro/ENGINEER will prompt the user with this message and highlight all of the unsolved vertices in red. As a default, the DIMENSION menu will be activated as a clue to add dimensions. The user can then Dimension or Align the highlighted entities or endpoints to fully constrain the section entities and regenerate the section successfully. Users may also run into a situation where they believe that the section is truly underdimensioned, but it regenerates successfully anyway. This is a function of implicit information, where sketcher makes certain assumptions depending on the creation of the section entities, their lengths, relative locations, zoom ratio, and Sketcher accuracy.
If there is too much dimensional information, Pro/ENGINEER solves the section and prompts the user with this message. The dimensions that are "extra" are then highlighted in red and the Delete menu is activated implying that the dimensions are not necessary and should be removed. In most cases keeping extra dimenions is unnecessary because they cannot be modified to change the feature and/or part geometry. If the user needs these for display and/or reference purposes, then a Ref Dim should be created in their place.
Eventhough a section may be fully dimensioned relative to each sketched entity, if it is not the first feature of a model, it still needs to be located with respect to the rest of the geometry. For example, creating a Solid Protrusion on a model that contains only default datum planes will require those sketched entities to be dimensioned relative to themselves, and also positioned relative to the datum planes. A circle would need a diameter or radius dimension, for the sketched entity itself, and a dimension or alignment which located that entity with respect to a horizontal and a vertical datum plane.
The feature being created requires the sketched entities to form a closed loop. A Revolve feature is one example that requires a closed contour of section entities.
The feature being created requires the sketched entities to form a single open loop contour. A Rib feature is one example that requires an open loop of section entities.
This message is just a warning that prompts the user that the endpoints of a sketch have not been explicitly located with respect to the other section entities or model geometry. This is a message that should be cleared by defining the open vertices more fully.
This message is specific to blend features. Rotational and General blends require a local coordinate system to be created in the section of the features for locating each subsection with respect to one another as they rotate and/or translate.
This message pertains to users that are utilizing Redefine to change the section of a feature that has dependent copies. If this occurs, the children must be removed using Delete from the FEATURE menu, or changed from being dependent with Make Indep from the MODIFY menu.
This error message informs the user that the section, in particular the highlighted arc, cannot be solved with the present constraints. This usually appears after dimensions that locate an arc are modified. The previously regenerated dimensions need to be restored and the dimension scheme must be reviewed.
This message is specific to blend and sweep features. If the sub-sections of blends are open loop contours, the start point must be at one end of the chain. If the trajectory of sweeps are open loop contours, the same applies.
This message is specific to blend features. This type of feature must have at least two (2) sections. Parallel and general blends will prompt the user for the extruded distance between each section. Rotational blends will follow the user defined rotational angle between each section.
This message is specific to blend features. It means that the number of entities must be the same for each sub-section. The sub-sections are switched by choosing Sec Tools Toggle. Entities like Centerlines and Construction Circles do not count towards this number. Only entities that will convert into geometry when the section is regenerated and the feature is finished are attributed to this message.
The best example of this requirement is a blend from a quadrilateral loop, square, to a circular loop, circle. The first section has four (4) entities and the second has only one (1) entity. The second section must be broken up into the same number of entities as the first. This can be done in a few ways. The circular section can have two centerlines added and then the circle can be broken up by using Geom Tools Intersect. By selecting each quadrant of the circle and each centerline, the user can divide the circle into four segments. Another method is to sketch the circle as four individual arcs.
This message pertains to users that are using Redefine to change the section of a feature that has children. If a sketched entity is selected for deletion, and this warning is given, it means that another feature, a child, directly references the entity. The proper method for removing this entity and creating another in its place is to first sketch the new entity to be used. Instead of using Delete, use the Replace selection under Geom Tools.
This message indicates that the sketch includes one or more relatively small entities which cannot presently be regenerated. One solution may be to simply enlarge the Sketcher window such that the "small" entities are more clearly visible. This may be accomplished by zooming in on the existing sketch as well. In instances where this problem cannot be resolved with these methods, an alternative may be to first create a sketch excluding the problem entities and regenerate the simplified feature. Then, relatively small features like rounds and detailing cuts may be added as separate features later. Sketcher accuracy may also be modified to enable Pro/ENGINEER to regenerate these relatively small entities.
Pro/ENGINEER extends line entities over the selected centerline, maintaining one segment. If there are dimensions on the mirrored lines, the dimensions will "stretch" to define the new entity length. Arcs, conics, and splines are broken into separate entities.
Sketched entities can be re-positioned through the Move command in the GEOM TOOLS menu. The selected segments can be translated and/or rotated in 90 degree increments about a user defined center point.
Several sketched entities can be re-positioned at one time using the Drag Many option in the MOVE ENTITIES menu. Their relative position to one another will be exactly as before the move.
The Use Edge and Offset Edge options in the GEOM TOOLS menu will create sketched entities by duplicating the edge definition onto the sketching plane, and automatically aligning to the geometry of the model.
Entities created through Use Edge and Offset Edge are automatically aligned to the model geometry they reference and do not require dimensions. The endpoints of the entities will also be aligned to the endpoints of the edge.
The Replace menu selection in GEOM TOOLS is used when altering feature sections through Redefine. If an entity is selected for deletion, and it is referenced by other features, the following prompt is issued : WARNING: This entity is referenced by other feature(s). Continue? [N]: Entering "Yes" will delete the entity and require redefinition of the child. By entering "No", the user can sketch a new entity to take the place of the entity being deleted. By using Replace, the reference required by the child will be maintained,
The sketching plane and horizontal reference plane used to orient a section can be changed through the Restart command in the SEC TOOLS menu. This will require that any sketched entities be recreated in the new section, but the user does not have to start over from the FEATURE menu and select the feature type and attributes again. Any entities that were sketched before the Restart can be salvaged by saving the section through Dbms, Save, and then retrieving the section with the Retrieve Sec command in the SEC TOOLS menu.
The Sketcher grid can be changed from the MODIFY GRID menu. It can be toggled on and off from the Grid On/Off command. The type of grid can be changed between Cartesian and Polar. The spacing and angle can be set with Params.
Arcs cannot be dimensioned explicitly with an arc length. This information can however be determined through Sec Info from the SEC TOOLS menu.
Sketcher accuracy, adjusted through Sec Tools, Set Up, Accuracy pertains only to the section in which it is changed. Every section has its own value and Pro/ENGINEER remembers the value for each separate section.
Two dimensional IGES data is brought into a Pro/ENGINEER feature section by selecting Sec Tools, Interface, Import, IGES.
Sketcher is a two dimensional utility, thus three dimensional information cannot be imported. If the data is necessary in Sketcher mode, Import the IGES file into Part mode, create a 2D view of the model in Drawing mode, then Export a new 2D IGES file, and Import that data into Sketcher. If the information is three dimensional, the following warning will be issued : IGES file contains 3D section. Cannot read 3D sections into sketcher.
Section entities imported through the INTERFACE menu of Sketcher mode must be dimensioned. If there is too much detail to dimension, import the IGES data into Part mode and Use Edge on the import feature when in Sketcher.
No, the grid is not plotted with the section entities and model geometry.
If the arrow head on the start point is in the wrong direction, it can be changed by using Sec Tools, Start Point. Select the desired point with Query Select and accept the Next choice.
Sections that have been saved to disk or are In Session can be retrieved and used in sketches of other features. Retrieve Sec will display the desired sketch in a sub window for preparation. The section can be rotated and scaled as it is placed into the active section. This is extremely helpful in cases where many features have the same or similar cross sections.
When toggling between sub-sections of blend features, the active sub-section will have entities highlighted in cyan. The entities that belong to other sub-sections will display in gray, hidden line color. If nothing is highlighted in cyan, the user has toggled to a new section that has yet to be created.
DXF files may not be directly imported into Sketcher. However, DXF files may be imported into a drawing. Once the data has been imported, an IGES file may be created and the IGES file may then be imported into Sketcher via the Interface option on the Sec Tools menu.
TIFF files may only be imported into drawings. Unlike imported IGES data, imported TIFF data does not export to an IGES file and, therefore, cannot be indirectly imported into Sketcher like DXF files..
Place Section is only available while creating a feature. If Sketcher is invoked by itself, the Place Section selection will be greyed out.
Send comments to webmaster@ptc.com
Copyright © 1995 Parametric Technology Corporation
,128 Technology Drive, Waltham, MA 02154. All rights reserved.