Use the Geometry dialog box to specify what features are to be simplified. Click Simplification and then, in the Options group, click Geometry to display the Geometry dialog box containing the following:
• Owner: Specifies the owner of the simplified model.
• FeatName: Specifies a name for the simplified part/assembly.
• Remove Blends: Click this check box to remove blends and chamfers with a radius or distance smaller than that specified in the MaxRadius field.
• Remove Helix Faces: This check box specifies whether or not to remove helix faces. Helixes with a diameter smaller that specified are removed.
• Remove Features: Use this group of check boxes to specify whether or not to remove pockets, bosses, slots, and ribs.
• Size Limitation: Use this group of fields to set size limits:
◦ Height: Specifies a value for how far a convex element (boss or rib) protrudes out of the base faces that contain it. This also affects combined boss/pockets such as when a boss is located within a pocket and protrudes over the base face of the pocket.
◦ Depth: Specifies a value for how deep a concave element (slot, pocket) penetrates into the base faces.
◦ Diameter: For each feature of the types boss/pockets/ribs/slots the system calculates a reference diameter by dividing the length of the cross section loops of the feature by pi. This makes it easier to specify value limits for features with circular cross-section like through holes. For non-circular cross section features the diameter is an approximate value representing a circular feature of similar size. For ribs and slots the cross section path is the sum of the end loops on both sides.
◦ Box Size: (Box Extension) This measure describes the maximum extension of the box of the simplification feature.
• Preview: Previews the selected faces.
• Check: Use this check box in any of the above modes to tell the system to check for validity. If a body check detects a corrupt part, that part is not simplified.
When setting limits, note the following:
• If no limits are chosen, all detected elements of the specified type are removed.
• If a limit is active and a feature candidate exceeds the limit value, the feature is kept.
• The parameters specified in the Geometry dialog box are only approximate measurement values. They can be used to specify an initial level of detail for the simplification. If the parameters do not match a specific situation, the faces option is taken and overrides the general parameters.
To set face options,
Click Simplification and then, in the Options group, click Faces to display the Faces dialog box containing the following:
• Keep Faces: Specifies a list of faces keep. A candidate feature/blend that contains such a face is not removed.
• Rem Faces: Specifies a list of faces to be removed. If a candidate feature contains such a face, it is removed even if the general geometric size parameters appear not allow for its removal.
If a face is selected that is not contained in a candidate feature, it is not removed.
• Preview: Previews the selected faces.
The settings you make here override the geometric parameters for selected faces.
To set structure options,
Click Simplification and then, in the Options group, click Structure to display the Structure dialog box containing the following:
• Assembly: Specifies the name of the assembly to be simplified (this is also the owner of the simplification).
• FeatName: Specifies the name of simplification definition.
• Keep Parts: Specifies a list of parts to be kept (see the note below).
• Rem Parts: Specifies a list of parts to be removed (see the note below).
• Remove Small Parts: This check box tells the system whether or not to remove parts less than a certain size as specified by the MaxSize value. This option applies to all parts in the assembly.
• MaxSize: Specifies the maximum size that a part needs be if it is to be included in the simplified assembly.
• Remove Hidden Parts: This check box tells the system whether or not to remove hidden parts (these are parts that are hidden in all 6 main views). Removing hidden parts has the advantage of improving system performance because there are less parts to be processed. This option applies to all parts in the assembly. This option is most effective when many parts are contained within a housing.
• Preview: Previews the simplified assembly.
• Original: Displays the original assembly view (similar to undoing the preview mode).
Overrides settings made in Remove Hidden Parts and Remove Small Parts.
To set merge options,
Use the Merge dialog box to specify what merge conditions are to be applied when simplifying an assembly. Merge parameters only apply if the merged structure has been selected in the Execute dialog box. Click Simplification and then, in the Options group, click Merge to display the Merge dialog box containing the following:
• Assembly: Specifies the assembly to be simplified.
• FeatName: Specifies a name for the simplification definition of the assembly.
• Allow Non-Manifold: This check box specifies whether or not to allow non-manifold edges (not manufacturable).
• Simplify After Merge: This check box specifies whether or not the resulting parts are to be further simplified.
• Check Merge Result: This check box specifies whether or not to do additional checking during the merge operation (this can reduce performance).
• Assy/Part: This box lets you specify several separate assemblies or groups. These groups are processed separately during the merge operation in order to have user-controlled non-connected subparts that can be positioned independently. Use the Select dialog box to select parts and assemblies to be included in the operation.
To set miscellaneous options,
Click Simplification and then, in the Options group, click Misc to display the Misc Options dialog box containing the following:
• Keep Visible Faces: Specifies whether or not to keep all visible faces. Part simplification is not done on detected candidate features that contain a visible face.
• Check Self Intersect: A simplification feature is not removed if the result was self-intersecting.
• Remove Hidden Parts 1: Checks for hidden parts before part simplification.
• Remove Hidden Parts 2: Checks for hidden parts that become hidden as a consequence of part simplification. This is easier to understand if you consider a part that contains several holes or slots that allow you to see inside the part. Strictly speaking, these internal parts are not hidden, that is, until the holes are removed.
• Keep Removed Elems: Specifies whether or not to keep removed faces as independent face parts for graphical feedback and result checking.
• Detect New Clashes:
◦ On: Clashes that are generated due to the simplification operation are marked in such a way that a drawing is created so that the clashes are correctly visible.
◦ Off: New clashes are not detected or made visible.
• Gen Mass Props: Specifies whether or not to automatically calculate the mass properties of the original before simplification and to assign these values. (As seen in the Part / Assembly dialog box.)
• Accuracy: Specifies an accuracy (as a percentage) for the mass properties calculation.
To set highlighting colors,
Click File > Settings > Simplification Color Settings. Use the Hilite Colors dialog box to set the highlighting colors during the simplification operation. Change the color in the usual manner by clicking the option and choosing a color from the color selector. The highlighting options are:
Geometry to display the Geometry dialog box containing the following:
Faces to display the Faces dialog box containing the following:
Structure to display the Structure dialog box containing the following:
Merge to display the Merge dialog box containing the following:
Misc to display the Misc Options dialog box containing the following:
Simplification Color Settings. Use the Hilite Colors dialog box to set the highlighting colors during the simplification operation. Change the color in the usual manner by clicking the option and choosing a color from the color selector. The highlighting options are: