When should a shell feature be added to a model?
How can a shell feature be created on a model that consists of only surface features?
How can the volume of material which a shell feature removes be measured?
How can a shell feature be created on a part that has a merge part contained within the geometry?
How can a shell feature have multiple thicknesses?
When should draft features be added to a model?
In which direction will a surface be drafted?
How can a surface be added or removed to a draft feature?
Does the section for a sweep created with the option Add in Fac require a closed section?
What functionality does the Merged Ends selection offer?
How can a sweep be created along a 3-D curve created from datum points ?
Why does the message "Z values reset to zero" appear when trying to create a spiral trajectory?
Why does the message "Radius of curve too small" appear upon sweep feature creation?
How can the actual length of a sweep features trajectory be measured?
How can the start point a sweep feature be located along the spine, rather than at an endpoint?
What is the proper way to utilize a graph feature?
How can a "3-D" sweep be created?
What is the difference between the "spine trajectory" and the "X-vector trajectory"?
How can the trajectories of a sweep be changed without recreating it?
What is meant by "Cannot intersect sketching plane with trajectories"?
What is "trajpar" and how is it used?
How can the length of any sweep trajectory be measured?
Why does the message "Radius of curve too small" appear upon sweep feature creation?
Why would a swept blend feature result in twisted geometry?
How can sections be added or removed from a blend feature after the feature has been created?
Warning: Offset surfaces are self intersecting.
Warning: Unattached Cut (or) Warning: Unattached Protrusion.
During shell feature creation, the external geometry is
offset inward. When this happens, Pro/ENGINEER may try to remove some of the
external surfaces in order to create the correct internal
geometry. Pro/ENGINEER shell features can not remove
spline surfaces, filleted
surfaces which are adjacent to one or more spline
surfaces or surfaces which become self intersecting due to the offset
value from the existing model geometry. Smaller offset values may enable
the shell feature to be successfully created since the resulting geometry
does not require a surface removal. Select Info, Surf Analysis,
Minimum Radius to verify if a shell feature can be created from a
selected surface; the minimum radius value returned is the maximum offset
value of a shell feature for that geometry.
*When should a shell feature be added to a model?
The shell feature should be added once all of the features that need to be included in the shell have been added to the model.
A shell feature only shells the solid geometry created by previous
features in the regeneration list. Additional solid features can be
inserted to regenerate before the shell after the shell has been created.
Likewise, the shell feature can be reordered to regenerate before or after
selected features as the user desires.
*How can a shell feature be created on a model that consists of only surface features?
Pro/ENGINEER will not allow a shell feature to be created on a model that consists of only surface features. Three alternative techniques can be used to create offset surfaces on a surface model.
There are two techniques that can be used to measure the volume of a shell.
Technique One:
Pro/ENGINEER will allow a shell feature to be created on a part that has a merge part contained within its geometry. It is important to save the merge components on disk for future reference since Pro/ENGINEER may require the models to update the model geometry at a later point.
*How can a shell feature have multiple thicknesses?
Pro/ENGINEER will allow shell features to be created which consist of multiple thicknesses. After selecting one or more surfaces to be removed for the shell feature, Pro/ENGINEER will prompt for a value for the shell thickness. Once the shell thickness has been specified, model surfaces can be selected which will be offset at a value other than the original shell thickness. Pro/ENGINEER will prompt for a shell thickness at each of the selected surfaces.
*If certain desired geometry cannot be created due to a shell feature failure, What other alternative technique can be used to create the offset surface geometry?
The following technique can be used to create the offset surfaces should the shell feature fail:
Draft features should be added to the geometry as soon as the model contains all the features that will be included in the draft.
*If a draft feature regenerates unsuccessfully, what is the best feature to create which would represent a draft?
If a draft feature cannot be created as a draft feature then the desired geometry can be created as a sweep using the following technique:
During creation of a draft feature, Pro/ENGINEER will prompt for a draft angle. The following "right-hand-rule" can be used to determine the rotational direction of the angle:
After a draft feature has been created, there may be surfaces which have been omitted or surfaces that must added to the draft feature. These surface can be added or removed by selecting Feature, Redefine, References, Dft Surfaces, Add or Remove and select the new surfaces to add or remove.
*What is a split draft?
A split draft is a feature that will draft a model in one direction on one side of a neutral plane and in the opposite direction on the other side of the neutral plane. This is very useful when creating parting lines for molded models.
*What is a curve driven draft?
A curve driven draft is a draft feature that will follow a datum curve selected on the model geometry; the datum curve must lie on the surfaces being drafted. If the datum curve that the draft is to follow does not lie in a plane, it will need to be created from the intersection of surfaces or created by projecting the datum curve onto the surfaces being drafted. The tangent of the datum curve cannot be parallel to the normal of the reference plane at any location along the length of the curve.
If the trajectory of a sweep feature is a closed loop the feature can be created with the Add in Fac option. A sweep feature created using Add in Fac can not have a closed section. Pro/ENGINEER will automatically close the section by adding top and bottom surfaces which close the feature.
*What functionality does the Merged Ends selection offer?
The Merged Ends option will extend the ends of the sweep such that it intersects the existing solid geometry. The sweep will only merge with the existing part geometry at the endpoints of the sweep's trajectory which are attached to the part geometry.
*How can a sweep be created along a 3-D curve created from datum points?
A sweep feature can not be created along a 3-Dimensional datum curve created Thru Points, From File or From Equation.
For more information on creating a 3-dimensional curve which can be used
in a sweep feature refer to Suggested
Technique for Creating a Spring as a Base Feature.
*When making a spring feature, why must the trajectory be sketched instead of selecting a spiral curve?
As a section is swept along a spine in a swept feature, the
sketching plane of the section will always be normal to the spine; the sketching
plane can still rotate around the spine however. A reference is needed to
orient the sketching plane as it is swept along the spine. A 3-dimensional datum
curve created Thru Points, From File or From
Equation does not have a reference to orient the sketching plane.
A datum curve created using Intr. Surfs, Projected, formed,
or Sketched will have a reference which can be used to orient the
sketching plane.
For more information on creating a 3-dimensional curve which can be used
in a sweep feature refer to Suggested
Technique for Creating a Spring as a Base Feature.
*Why does the message "Z values reset to zero" appear when trying to create a spiral trajectory>
This message is given in the following situations:
When creating a section for a variable section sweep, the section size cannot exceed the radius of curvature of the trajectory. This situation will cause the sweep feature geometry overlap onto itself creating invalid geometry. One of the following can be done to correct the problem:
The length of a sweep feature can be measured by selecting Info, Measure, Curve/Edge, Length, Query Select and selecting the entire trajectory.
*How can the start point a sweep feature be located along the spine, rather than at an endpoint?
A sweep features section can start in the middle of a spine if a datum point created by selecting Feature, Create, Datum, Point, Crv X Surf exists in the middle of the trajectory. To create this datum point, select the curve in the trajectory where the point is to intersect and then select a plane or surface which intersects the curve at the location where the section is to be sketched. Upon creation of the sweep, Pro/ENGINEER will prompt where the section is to be sketched and the point created using Curve X Surf can be selected by selecting Next from the menu. When the point where the section to be sketched highlights, select Accept.
Graph features must follow 2 specific criteria in order to work correctly:
The suggested technique to create a variable section 3-D sweep is to create a sweep feature along a datum curve that has been created at the intersection of two surfaces. A sweep can not be created along a 3-dimensional datum curve created using Thru Points, From File or From Equation.
*What is the difference between the "spine trajectory" and the "X-vector trajectory"
The spine trajectory is the trajectory to which the section will remain normal. The x-vector is the trajectory to which positive X-axis of the section will point towards.
*How can the trajectories of a sweep be changed without recreating it?
A sweep feature can be redefined by selecting Feature, Redefine. Select Section from the REDEFINE menu. A SECTION menu will appear which will allow you to redefine any of the selected or sketched trajectories that have been used to create a variable section sweep. It is important to remember that the newly sketched or redefined trajectory should contain the same number of sections as the old trajectory, and should follow a similar path. A violation of these could result in a failed feature.
*What is meant by "Cannot intersect sketching plane with trajectories"?
The error message "Cannot intersect sketching plane with trajectories" will be returned while creating a variable section sweep feature if the sections sketching plane (which is normal to the spine) does not intersect all of the trajectories used to create the sweep at the start point of the spine.
*What is "trajpar" and how is it used?
Trajpar is a value normalized along the spine of a variable section sweep. The value can vary from 0 to 1 as
the section is swept. Trajpar is a trajectory parameter which can be used in a sketcher relation to
"map" a graph or any functional equation along the variable section sweep feature. By using trajpar
in a sketcher relation the driving dimensions in the section can be varied as the section sweeps along the spine.
*How can the length of any sweep trajectory be measured?
The length of any sweep trajectory be measured by selecting Info, Measure, Curve/Edge, Length, and Query Select the entire trajectory for measuring.
When sketching sections for a swept blend feature, verify that the start points of each section correspond to the vertex on the preceding section. Pro/ENGINEER tries to "line up" the start points when creating the feature. If the start points are not aligned properly, the resulting geometry may twist between blend sections.
*Will small surfaces created when a swept blend feature is created effect the geometry and is there a way to minimize these extraneous surfaces?
The number of segments in a section or trajectories will effect the number of surfaces created in a swept blend feature. When specifying sections or trajectories for a Swept Blend feature, utilize sections and trajectories which have as few non-tangent segments as possible. Spline segments can be used to minimize the number of surfaces in areas where a sketched entity may intersect another sketched entity and the intersection may not be tangent. Tiny surfaces created in a general blend could effect the model geometry in that when subsequent features are created on top of the blend feature (ie. rounds, drafts, chamfer) there may be more difficulty creating these features.
*Why does Pro/ENGINEER state that a coordinate system is missing when sketching sections for a blend feature when a coordinate system exists in the model?
Pro/ENGINEER must reference a sketcher coordinate system when creating a general blend. This coordinate system can be created by selecting Sketch, Adv Geometry, Coord Sys and placing the sketcher coordinate system on the section.
*During blend feature creation, how can a section be sketched along a trajectory if no vertex exists at the desired location?
During the creation of a blend feature, Pro/ENGINEER will only prompt for a section to be created at the endpoint of each segment of the spine. It may be desire that a section be sketched along the spine at a location where an endpoint does not exists. To create a point which can be used to specify additional section locations along the spine, use the following technique:
A section can be added to the original swept blend feature only if the feature was created using Select Section to define the blended sections. If the sections were sketched, the feature must be recreated to remove or add sections to the blend.
As of Release 16.0, Pro/ENGINEER allows for creation of both simple and advanced rounds. A simple round uses the default shape and transitions, while an advanced round allows the shape, spine, and transitions of the round to be specified. With a single advanced round, you can now create several different types (i.e. edge chain, surface-surface, etc.) of rounds and connect them with user-defined transitions. Each round type specified within an advanced round is known as a round set.
This message may occur during the creation of shell or offset surface features. This message typically indicates that the surface being offset has a high degree of curvature causing the geometry to close in upon itself during the surface offset. Pro/ENGINEER will not create this geometry.
*Warning: Unattached Cut (or) Warning: Unattached Protrusion.
There are a number of causes for this error message, and each cause may be addressed differently.
If the protrusion/cut is extremely small relative to the overall size of the part, try increasing (smaller number) the accuracy of the part. This will allow for smaller features to be created, as either cuts or protrusions.
Check to see if the proper type of cut was applied. If a surface trim is applied to solid geometry, or vice versa, then you will get this error message. Match surface trims with surface features and solid cuts with solid geometry.
If the protrusion is a swept feature redefine the section and unalign any alignments or edges referenced using Geom Tools, Use Edge. Dimension the sketch as much as possible to the cross hairs of the trajectory. Also, delete any extra dimensions from the sketch.
If the protrusion is a solid created from a quilt, ensure that all edges of the quilt are magenta. If there are yellow edges, patch them up with other extended, trimmed or boundary surfaces, merging them into one quilt.
If a Geom Check indicates that there are tiny edges present because of an unattached cut, re-orient the cut, or create the cut in a different method to eliminate the tiny edges.
If the feature is a member of a radial pattern, redefine the leader of the pattern so that it does not reference the circular edge or cylindrical surface in any way. The section should reference only the axis of the cylinder, or the vertical reference plane that is to rotate with the protrusion (usually a make- datum).
A spline can be defined by the following means:
If either the envelope of the model or the model accuracy value increase, Pro/ENGINEER will regenerate the model less accurately which may result in geometry errors. If a model requires small edges or surfaces with respect to the overall size of the model then the model accuracy value may be decreased to allow for shorter edges and surfaces to be successfully regenerated. Decreasing the model accuracy value will cause regeneration time to increase (the geometry is evaluated more accurately) and may cause geometry which previously regenerated successfully to have geometry errors.
Note: It is recommended to use the Pro/ENGINEER default model accuracy value of
0.0012. If possible, it is recommended to resolve geometry errors by
redefining the model geometry.
*What is a merged part?
Send comments to webmaster@ptc.com
Copyright © 1995 Parametric Technology Corporation
,128 Technology Drive, Waltham, MA 02154. All rights reserved.