Wednesday, November 5, 2014

Siemens NX Tutorial III - WAVE Engineering

General Re-linker - Automatic:

Path: Assemblies tab > More > WAVE gallery > General WAVE Relinker


The General Relinker can be used to automatically or manually relink geometry when links may be broken due to replacing components or modeling changes. The system relies on attribute names applied to the Target and Source objects when automatically relinking.

Prerequisites:
In order for the links to automatically update the Source and Target objects must have attribute names assigned. These names must be defined in the settings area of the General Relinker dialog.


Step 1: Open the file auto_relink_assy\auto_relink_assy.prt.


Step 2: For the system to find the Source and Target geometry to update any links attribute names must be assigned to the geometry objects. These names are then searched from the Settings pane of the General Relinker dialog.


Step 3: Make the case_2 the displayed part and select the indicated face; you may need to set the selection filter to face.


Step 4: Right-click and select Properties to display the Properties dialog. Select the General tab to display the name of the face.


This is the name used for the Source Object Filter.


Step 5: Make cover_01 the displayed part and select the indicated face. Make sure it is the linked face.


Step 6: Right-click and select Properties to display the Properties dialog. Select the General tab to display the name of the face.


This is the name used for the Target Object Filter.


Step 7: Make auto_relink_assy.prt the work and displayed part and select Home tab Assemblies group Components Drop-down > Replace Component and select the case_2 component. Replace it with filter_case.prt.


Step 8: Select Assemblies tab More > WAVE gallery General WAVE Relinker to display the General Relinker dialog.


Step 9: Set the Source Scope and Target Scope to Parts in Assembly.
Step 10: Make sure the Target Object Filter is set to *IN and the Source Object Filter is set to *OUT.
Step 11: 
Click Relink to automatically relink the geometry. The links should all automatically relink.


Step 12: 
 Click Update Session in the Update pane to update the models. The solids update to the new links.

Step 13: Click OK from the General Relinker dialog.

Source Scope and Target Scope:
You can filter for parts to define where the linked objects are from (source) and to (target).

Parts in Session
All parts open in your current session will be checked for an applicable attributes and links.

Parts in Assembly
Only the parts in the current assembly will be considered for relinking.

Work Part
Only the current work part will be used for any target objects to relink.

Selected Parts
When active the select component option displays and you can individually select the target components to relink.

Relink:
 When you click Relink any objects included in the Source and Target scope that can automatically relinked display in the Link Browser. 


Any objects that fail display as a broken link.

Update
From the Update pane of the dialog you can Break Wave Link or Interpart Expression on selected links and Delay Update on Manual Relink.

Update Session:
 Click Update Session to update the recognized links and the models.

View Feature Failure:
 If a feature fails to update due to the relinking process you can review the failure with the View Feature Failure dialog.

When a failure occurs you can use the option on the dialog to help isolate and hopefully fix the problem.

 Take Me to This Part makes the selected component the Work part.

 Roll Back to This Issue makes the component the Work part and makes the offending feature current.

 Re-Test This Issue retries to create the feature after you have made an edit.

 Create Report outputs a web page document (.xml) that you can review later or forward to the correct user.


The Feature Details box in the Information pane can be used to review the details when a feature fails.


Settings: The system uses attribute names to recognize the linked geometry in the source and target files.


You can define the link names and filters for the system to search through. The default names can be controlled from the customer defaults.


Link Option: You can choose to only update Interpart Expressions, WAVE Geometry or Both.

Include Non-broken Links: If enabled the system will show all links when executing a relink.

Include Suppressed Components: When active any suppressed components will be included, although they will not update until they are unsuppressed.

Face Normal/Curve Direction Adjustment: When active the system automatically sets the curve or face normal if necessary.

Tips
  • When naming faces you want to be careful to name the face of the linked object. If you name the linked object, the relinker will not recognize the name. This is rather confusing but a linked face object has a face. In this example item number 4 in the QuickPick is the Face of the Linked Face (0) feature.

  • When naming faces used in the relinker, it is important to make the part the displayed part. Naming the faces in the context of the assembly (making the part the work part) are not recognized by the relinker.
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General Rilinker - Manual:
PathAssemblies tab > More > WAVE gallery > General WAVE Relinker

The General Relinker can be used to automatically or manually relink geometry when links may be broken due to replacing components or modeling changes. The system relies on attribute names applied to the Target and Source objects when automatically relinking.

Prerequisites
  • In order for the links to automatically update the Source and Target objects must have attribute names assigned. These names must be defined in the settings area of the General Relinker dialog.

Step 1: Open the file manual_relink_assy\manual_relink_assy.prt.


Step 2: Select Home tab > Assemblies group > Components Drop-down > Replace Component and select the filter_case component.


Step 3: Click Browse and select the small_case from the same folder the assembly was in and OK to complete the replacement.



Step 4: Select Assemblies tab > More > WAVE gallery > General WAVE Relinker to display the General Relinker dialog.



Step 5: Set the Source Scope and Target Scope to Parts in Assembly.



Step 6: In the Settings pane, make sure the Target Object Filter is set to *IN and the Source Object Filter is set to *OUT.



 Click Relink to automatically relink the geometry. If any links break the "broken link" symbol will display next to the link.
Review the description and see that the link did not have a name applied.

It is possible that the link is not broken but the names did not match up. In that case, an "exclamation point" symbol will display next to the link.
Step 8: Right-click on the failed link and select Manually Relink.



Step 9: The WAVE Geometry Linker displays and you can select the new source geometry.



Step 10: Hide the filter component and select the inside lip of the small_cover to update the linked geometry.



Step 11: Click OK from the WAVE Geometry Linker to return to the General Relinker dialog.



Step 12: The Model should update to the new geometry.


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Design In Context:
When designing in the context of assembly, WAVE can be a tremendous time-saver. WAVE lets you link geometry in order to avoid duplicating features in multiple part files. Common techniques include creating linked sketches for defining profiles, linked points for positioning features, linked faces for trimming operations, and linked mirrors for creating opposite hand parts.

Profiles
WAVE is an excellent tool for linking curves or sketches to create profiles in interfacing parts. This associativity eliminates the need to make measurements, refer to drawings, or create numerous interpart expressions to match two profiles.
Consider the housing in the following figure.

To make a cover for this object, you must create a plate with a matching profile. You can do so by creating a sketch and extruding it or use the feature-based technique of creating a block, four pads, and several blends. In either case, it requires looking up the values of the housing profile in order to create the correct size of profile for the cover. To link the parts parametrically, you need several interpart expressions.
Perhaps a simpler solution is using the WAVE Geometry Linker dialog to create linked curves of the housing edges and extruding them to create the cover. This design is much easier and faster than the previously mentioned methods.

With a little planning, you can simplify this method even more. For example, you could model the housing profile as a sketch. The WAVE Geometry Linker dialog lets you link the entire sketch. In order to design in this manner, the sketch must be visible in the assembly. In this assembly, a reference set named 'BODY' displays only the solid body. The sketch is made visible in the assembly by replacing the reference set to 'Entire Part.' Now you can use the WAVE Geometry Linker dialog to create a linked sketch in the cover part file. The advantage of creating a linked sketch instead of linked curves is that only one item is selected and only one feature created in the cover to represent the profile.




In this case, the sketch represents the outside profile of the housing lip. It is necessary to match the inside profile of the housing lip. Creating a single interpart expression and offsetting the profile provides an easy solution to this requirement. This expression links to the thickness of the housing lip, accommodating any future changes to the lip. Adding a clearance to the expression ensures the cover fits the housing. For example, if your expression reads "OFFSET=housing::THK," create a clearance by adding "+.5" to the expression. Consequently, the expression would read "OFFSET=housing::THK+.5."
Select Curve tab > Derived Curve group > Offset Curve to offset the profile, using the expression OFFSET as the Distance value. This command creates a feature, so the new profile is still parametric to the housing profile. 

Now extrude the offset profile to create the cover plate. This method takes less than five minutes and creates only three features. Make the holes by creating and extruding linked curves based on the edges of the existing holes on the housing. The entire model is now tied to the housing. If the housing profile ever changes in size the cover automatically changes also, retaining a 0.5mm clearance.

Positioning
An alternate method of creating the holes in the cover plate for the housing is to use linked points to position hole features. This method ensures the hole positions in the cover are the same as the housing. To link the size of the holes, use an interpart expression, as prepared for the offset of the profile.
Make the cover plate the Work Part, then use the WAVE Geometry Linker dialog to create linked points at the center of each of the housing holes. 

Then, use the Point onto Point constraint to create and position Hole features, aligning the center of the holes with the linked points.
Timming:
Another fundamental use for WAVE geometry is during trimming operations. You can link datums, faces, or bodies to another part file to use for trimming material. This method is useful when ensuring two interfacing parts fit together.
Consider the simple example of two intersecting shafts.

Create a single, linked face, then use Home tab > Feature group > Trim Body to trim the solid body. When using this feature, it is important to remember that the trimming face must always extend beyond the solid body.
This technique can be especially useful when the matching faces are hard to duplicate. Free form surfaces requiring several profiles and guide strings must be duplicated in the interfacing part. Not only can that be a lot of work, but when the surface is modified in one part, the same modification needs to occur in the second part.
The positioning of one model with respect to the other can compound the problem. Consider the following spaceball model. 

The button is carefully positioned in the assembly on two boss/pad features. A cutout in the cover is needed to match the oval-shaped feature on the button. The profile of this feature is not too difficult to duplicate. However, the position of the button in the assembly makes creating this cutout a challenging task. Its orientation about three axes to match the contour of the cover makes several datum planes and axes necessary to create the appropriate sketch defining the cutout profile.
WAVE solves the problem of duplicating the positioning of the cutout in the cover. It also sets the model up for easy modifications. Ergonomics studies might dictate the button change in size and position. By modifying the geometry in the button part file and the position in the assembly part file, the cover automatically updates.
Depending on the complexity, the user can link the solid of the button or the outer faces if it is created from several bodies.
Complete the process by selecting Home tab > Feature group > More > Offset/Scale gallery > Offset Face to add clearance between the cutout and the button. Use an offset value of -0.25mm to make the cutout slightly larger than the button. This operation can be done either before or after the trimming operation.
Mirror Body:
When there is symmetry in an assembly, use Mirror Body in the WAVE Geometry Linker dialog to create an opposite-hand model.
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In-Process Model:

WAVE functionality can be used to interactively manage the basic steps in the design process. A common application for this is the creation of a machined part and a related mold tool.




Castings and Machined Parts
When designing parts that are cast and machined, it is usually required to create a separate version of the part for both processes. An alternative parametric approach is to model the casting first, create a machining file which acts as an assembly node, and then add the casting as a component and 'promote' it (using Home tab > Feature group > More > Associative Copy gallery > Promote Body). This allows additional secondary features (such as drilling, machining, etc.) to be incorporated into the design. 

WAVE engineering, however, offers yet another alternate method of creating the machined part. The WAVE Geometry Linker dialog is used to create a linked body feature in the machined part file; the machined file can be at the assembly level as with the 'promote' method, or can be a separate child component (at the same level as the casting). Advantages are that WAVE is more efficient in memory usage, the part data loads quicker, and both versions can be accessed and viewed together.

For optimal visualization, a reference set should be created to include only the machined body when viewing the assembly.

Mold Cavity and Core:


Similar to creating a machined version of the part which is linked to the casting, WAVE can also be used to develop the tools for an injection mold. A linked body of a cast part can be used to trim the both cavity and core halves of a mold tool in separate parts created to represent them.



Because the designed part usually represents the finished size, a scaling operation can be performed on the linked body to account for shrinkage in the mold process.


This example has both the exact linked body and the scaled body in the same part file, so specific reference sets are helpful to visually distinguish them. A 'BODY' reference set could display only the original solid body in an assembly, and a 'SCALED_BODY' reference set could display only the scaled solid body.
The block part defining the tool can also reference interpart expressions if desired, and base its size on that of the original part. 
Either trim or subtract features can be used to complete the tool shape, as both retain the parametric link to the original part.
In parts with a complex parting line, a linked region of faces can be copied (instead of the entire body) for the parting development.
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Control Structures:
WAVE can aid in designing an assembly using the top-down method, which can be useful when there are complex relationships between components. By defining this relationship at the assembly level, you can avoid difficult positioning or mating problems.


Control Structures Example:
Consider a simple gear assembly. If you construct each gear individually, positioning them in the assembly can be challenging. Making changes to the gears requires that you reposition them. Even if you can mate the gears successfully, a number of interpart expressions will be required.
A better approach is to define the gears in a single sketch. This sketch is essentially a layout, defining the size and location of each of the gears in the assembly.

Basic gear principles define the dimensional constraints in this example. By taking this approach, you can modify the assembly in a single part file - the top assembly. You can easily modify the driving parameters of this gear assembly in the sketch or in the Expressions dialog.



To complete this design, you can now create the individual components based on the sketch. A linked curve was created in the part file for the drive gear and extruded to define the gear. Additional features were created to complete the design of the gear, which is repeated for each of the gears.




Note Note that the gears are modeled to the pitch diameter. To simplify the model, we did not model the gear teeth because their profiles only needed to be shown on drawings.
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Modelling Errors:

The most common errors encountered when using WAVE are caused by changes to the parent geometry of linked features. 


Changes to the Parent Geometry:

The Design In Context section explained how to construct a cover for a housing using linked geometry. The first approach involves creating linked curves based on the solid edges of housing and extruding them to create the cover plate. 


If the linked edges are consumed in any way (whether the edge is blended or a pad / pocket is added to the surface for example) The linked curves would fail because of the gap, and the cover will be full of errors as a result.


By changing the edges, the solid edge that you use to define the profile is modified. In this case, the solid edge splits into two edges with a gap between them. The first edge is the original edge - a parent to a linked curve feature in the cover plate. The second edge is a new edge that is not linked to the plate, which results in a large gap in the defining string of the extruded feature creating the plate. Depending on the Modeling Preferences theError during Update dialog or a warning alert may appear, noting that feature EXTRUDED(2) does not update because the defining string (the linked curves) is not closed. The best case outcome is when the extrude does not fail, but the feature is a sheet because of the open string.


Using the At Timestamp Option
In this situation, you can fix the error by editing the Linked Composite Curve feature that is the child feature of the modified edge. Activating At Timestamp allows you to select the feature to which the curve is to be linked. For example, selecting Home tab > Edit Feature group Edit Feature Parameters and picking the curve displays the WAVE Geometry Linker dialog.
Note that At Timestamp is inactive. Since this option is not active, the feature Rectangular Pocket (41) affects the linked curve.
Activating Fix at Current Timestamp allows you to select when the feature curve is to be linked. This example shows Simple Hole(40) selected. This is before feature Rectanguler Pocket (41) creates the gap, and the model updates.


It is important to realize when to use this option when using linked features. As design intent changes, you may need to change the status of this option to fix errors.
An Alternate Approach
Recalling the second possible method for constructing the cover, a linked feature was created based on the profile sketch of the housing. This approach results in a single linked sketch rather than twenty-four linked curves.


Using this approach not only makes creating the cover simpler, it also avoids the error caused by the pocket feature. Because the sketch, and not the edges, is the parent WAVE geometry, the defining string of the cover's Extrude feature remains intact. In addition, if the sketch is modified and curves are added and removed, the parent WAVE geometry is also changed.
In this case, planning how the housing was constructed helped model the cover. Using a sketch to define the profile, instead of exclusively using features, avoids using the solid edges as parent geometry to the WAVE features. Developing a careful strategy to follow your design intent is important.
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Delayed Errors:
A danger in using WAVE is that an existing error may not appear immediately. When an assembly loads, existing errors do not necessarily surface.


Delay Geometry, Expressions, and PMI Updates
Consider the error explained in the section Modeling Errors. If the assembly loads with the Delay Geometry, Expressions, and PMI Updates option active, the error does not appear. This result occurs because the housing part only updates. The rest of the parts in the session, which includes the cover part containing the error, do not update. 
Load Options
Many times, a modeling change is made when a single part file is loaded, but the assembly is not. The error does not appear immediately in this scenario either. Even upon opening the assembly, the error may not yet appear. Depending on your load options, the assembly can load without updating its components.

This result happens when the option Use Partial Loading is active and Load Interpart Data is inactive in the Load Options dialog.

Loading the WAVE data triggers the error. If Load Interpart Data is active when the assembly loads, even if partially, the Edit during Update dialog or a Warning Alert appears. 
You can also load the WAVE data by selecting Assemblies tab > More >WAVE gallery > Load Interpart Data. This command displays the Load Interpart Data dialog. Clicking either button on this dialog triggers the error.

Partial Loading
If the Use Partial Loading option is inactive, then the assembly and all of its components load fully. Fully loading an assembly also loads the WAVE data, regardless of whether the Load Interpart Data option is active, thereby triggering the error.
However, when the Use Partial Loading option is active and the Load Interpart Data option is inactive, none of the WAVE data loads. If no direct action is taken to load all of the WAVE data, then the data loads only for each component, as it is fully loaded. The caveat for this situation is that both the component containing the parent geometry and the component containing linked features must be fully loaded to trigger the error.
Designating a component as the Work Part or Displayed Part, fully loads it. Therefore, it is possible to load the assembly and change the Work Part to the cover and NOT trigger the error.
If one is not careful, the error may not be recognized for a long time. The error then causes major headaches for everyone involved, since more downstream features are created, either in the same part or in others. A possible snowball effect can occur, ending with someone having to deal with multiple errors at once.
Therefore, it is imperative to load all of the WAVE data for the assembly on a regular basis. You can do so by activating the Load Interpart Data option before opening or fully loading an assembly. If an assembly is already partially loaded, it can easily be fully loaded by selecting the assembly in the Assembly Navigator, then right-clicking and selecting Select Assembly from the pop-up menu. To complete the operation, right-click again and select Open > Component Fully.



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Circular Reference Errors:
Overview
A circular reference is an error that occurs when a child object is used to modify its parent. While it seems logical that one should not attempt to create this relationship, it is a common error when using WAVE to design an assembly.


Planning and Managing WAVE Data
The reason this error occurs is usually due to poor planning and/or model management.
Designing with WAVE requires careful planning to determine which parts are to be used to create others. With interfacing parts, one of the parts is chosen to contain a common feature and can be used to create WAVE geometry in the other. Additional common features should be created in the same part file to avoid creating a circular reference.
As more components are created in an assembly and as more WAVE geometry is created, it becomes harder to keep track of the WAVE links. If more than one designer is working with WAVE in a given assembly, it is nearly impossible to keep track of the links without WAVE management tools. This situation is when the WAVE control license pays off.
It is also important to understand that a change in the design intent may require major changes in the models, which could mean re-associating WAVE features to new parent geometry in order to avoid circular references or other errors.
The Circular Reference Error
When one loses track of the WAVE links in an assembly, it becomes easier to generate a circular reference error. For instance, existing edges in Part A are used to create linked curves in Part B. Part B curves are used to create new features and edges of these new features are then used to create linked curves in Part C.
This process can continue, creating several levels of both features and parts. Once any child object in any part is used to modify the parent geometry in Part A, the circular reference error appears.
Note Circular references will be used in the Part Management project at the end of this unit.
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File Management:
Using WAVE requires you to carefully consider the way you manage your part files and assemblies. Operations you might normally do to an assembly, such as renaming it from the operating system, can produce unexpected results.


Cloning
Cloning WAVE parts sound logical, but it is important to consider what is happening before doing so. The simple rule is that the child part must have the same action, retain or clone, as the parent. If you try to assign a different action to a child, NX automatically changes the action on the parent and notifies you of the change.

This behavior may seem inconvenient, but the alternative would cause either broken links or duplicated references.
The exception to this behavior is when the links span assemblies and not all the assemblies load in the Clone Assembly dialog. For example, if you clone a sub-assembly that has links to a top assembly, the links break in the resulting cloned sub-assembly. There is no avoiding this result, unless you clone the entire top assembly (probably not desirable), or add the cloned sub-assembly into the top assembly.
Suppressing Components
Suppressing a parent component does not break any of its WAVE links. However, changes made in the parent part file do not reflect in the child parts until the parent is unsuppressed in the assembly.

Renaming Part Files
You must be careful how you rename parts with WAVE links. If you rename an assembly from the operating system, the linked components still point to the original assembly name; they have no way of knowing that you renamed the assembly outside of NX. These links do not display as broken links; NX simply assumes that the parent assembly is not loaded. If you rename the assembly to the original name in the operating system, everything returns to normal.
If you use Save As on a child part without its parent assembly loaded, the link initially displays as unbroken. However, as soon as you open the parent, the links in the renamed part break. Unless you add the renamed part to the assembly, you cannot restore the links.
In summary, do not rename WAVE parts in the operating system and do not use Save As on a child part unless its parent assembly is loaded.
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Editing:
You will model the bracket to fit against a side member of a chassis member. Use linked faces to trim the geometry of the bracket, matching it to the member. Edit the bracket, noticing the way WAVE geometry is used and the problems that can occur.

  • The option Allow Interpart Modeling must be active in the Customer Defaults dialog.

Step 1: Open chassis_assy\chas sis_assy.prt. Make bracket_lca_lh the Displayed Part. Examine the linked geometry on Layer 6, noting its use in the model.


Step 2: Edit the PROFILE sketch, changing expression p1884 from 260 to 275 in order to lengthen the part. Update the model.

Depending on your preferences, you will see an information window telling you about failures that occurred or you may be presented the Edit During Update dialog displays.
If you received the information window, you only need note the failures. If you received the error during update dialog, the feature TRIM_SHEET(29) cannot update due to a non-manifold solid error. Click Accept Remaining to allow the model to update. 
There is a problem with trim sheet features use the linked faces to trim the model. That causes a failure of some downstream edge blends.
Step 3: Examine the model to determine why the trim sheet features failed.



The linked faces no longer extend beyond the solid, causing the trim sheet features to result in a non-manifold solid error. When trimming a solid body, the trim sheet must extend beyond the solid. In this case, the part was lengthened and now extends beyond the linked faces used to create the trim. 
Step 4: Make chassis_assy the Displayed Part and Work Part. Replace the reference set for bracket_lca_lh to the 'Entire part' in order to see the linked faces. Make bracket_lca_lh the Work Part and make layer 6 the work layer. Create the linked faces needed to update the trim features.

Step 5: Make bracket_lca_lh the Displayed Part. Create offset features for the two linked faces, using the expression THK as the Distance value. Select Home tab > Surface group > More > Surface gallery > Offset Surface to create the offset features. 


Step 6: Sew the linked faces to the existing sewn trim sheet. Sew the offset faces to the existing sewn trim sheet.

Step 7: Reorder the new features (all LINKED_FACE, OFFSET and SEW features) before the TRIM_BODY(29) feature. These six features must come before the TRIM_BODY(29)feature to correct the non-manifold solid error. Reordering causes all of the features starting at TRIM_SHEET(29) to update, including the out-of-date features.


Review: Modeling with WAVE geometry can be complicated, because you have to be aware of both the current model and any models containing parent geometry to linked features. Changes to these models can very easily trigger errors in downstream features. Carefully examine your model when making changes. Problems can arise even with features that appear unrelated or up-to-date.
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Part Management:
You will add a closeout plate to the bracket assembly. The plate interfaces with a sleeve, which must be modified to fit the plate. Then, load a bushing into the assembly. Observe when existing WAVE geometry and interpart expressions cause problems, because the assembly is improperly managed.
To understand the types of problems that can occur when using WAVE geometry and interpart expressions between parts shared between different users.

Step 1: Select File tab > Preferences > Assembly Load Options. Set Load to Structure Only, deactivate Use Partial Loading, deactivate Load Interpart Data, and click OK.


Open part_management\part_management without loading its components. 



Fully load the components bracket_lca_rh and sleeve_rear.


Step 2: Add the file plate_closeout to the assembly as a component. Change the reference set to 'PART,' set Positioning to Absolute, and place it into the assembly.


Step 3: Make sleeve_rear the Work Part. Hide the component sleeve_rear to view the face to link. Create a linked face to the cylindrical face of the hole in the component plate_closeout.


Step 4:
Make sleeve_rear the Displayed Part. Extrude the edge of the linked face 43mm in the -YC direction with an offset of 1mm, subtracting it from the solid body to create a groove the same diameter as the hole on the component plate_closeout.
The Extrude operation cannot be performed due to an error. A message window and the Information window both appear. If you did not get an error, you likely have the Delay Update toggle enabled. 
Step 5: If you do not have Delay Update enabled an error message appears stating, "There is an object which depends on itself." Click OK to continue. Examine the Information window and the Part Navigator for both sleeve_rearand plate_closeout to determine the cause of the error. 

To understand the cause of this error, you must understand the history of the part plate_closeout. The hole feature in plate_closeout is created by using a linked face, LINKED_FACE(2), as a trim sheet. This face is linked to the outer face of the part sleeve_rear. An additional feature, OFFSET(4), makes the hole in the plate smaller.
Not recognizing this existing interpart link, you created a linked face in sleeve_rear based on the cylindrical face of this same hole. Attempting to use the edge of this linked face to modify the outer face of the part sleeve_rear therefore causes the circular reference. 
Step 6: Make sleeve_rear the Work Part. Measure the depth of the desired groove by measuring the distance between the outer edge of the sleeve, and the edge of the linked face. 
Select Analysis tab > Measure group Measure Distance and select the two edges. The distance measures 7.0mm.
Step 7: Delete the linked face created in step 3.
Step 8: Create an expression named GR_DEP equal to the distance measured in the previous step.

Step 9: Create the desired groove by extruding the edge of the face 43mm in the -YC direction with an offset of -GR_DEP, subtracting it from the solid body.

Step 10: Make plate_closeout the Work Part. Edit the feature Offset Face(4) and replace the offset value with sleeve_rear::GR_DEP.

By replacing the 0.7mm value with the interpart expression, the original intent is achieved. The diameter of the groove on the sleeve is always the same as that of the hole on the plate. You can input the interpart expression in the widget or use the expression editor to create an interpart expression.
Step11: Make part_management the Work Part and select File tab > Preferences > Modeling. On the Update tab, Activate Errors and Warnings in the Edit During Update Dialog Appears on section.

Step 12: Load the component bushing.
Step 13: Examine the Edit During Update dialog and click Accept Remaining.

The REVOLVED(5) feature fails to update.
Step 14: Select Assemblies tab > More > WAVE gallery > Interpart Link Browser. Click Objects and in the Graphics window, pick both the solid body of the sleeve and the bushing. There is no interpart link in the bushing and the only interpart link in the sleeve is that with the plate.

Step 15: Designate sleeve_rear as the Work Part. List the expressions to determine if there are any interpart expressions.


Four interpart expressions reference the expressions DIA1 and DIA3 in bushing. Loading the bushing part updates these expressions and causes the feature REVOLVED(5) to fail. This result indicates that a change was made to the bushing part, because it was last loaded in the assembly.

Step 16: Use the Feature Browser to determine the parent of the feature REVOLVED(5). Select Menu > Information > Browser, pick REVOLVED(5). The INNER_PROFILE sketch is the parent feature.


Step 17: Designate sleeve_rear as the Displayed Part. Examine the INNER_PROFILE sketch to determine the cause of the error. 


The interpart expressions drive the diameter of this sketch outside of the solid body. The bushing is designed to fit inside of the sleeve. Its size change is causing the REVOLVED(5) feature to fail.

Step 18: Designate bushing as the Work Part. Change the expressions to the following parameters:
DIA1: 48.77
DIA248.26
DIA348.13
Designate part_management as the Work Part and examine it.

Review: When using interpart links and expressions in an assembly, part management is very important. Beware of the defined links and the way they reflect the design intent. Evaluate the intent behind these links often.
When multiple users are working in the assembly, management becomes even more important. If you do not communicate with one another about the interpart links that exist and the intent behind them, problems, such as the ones encountered in this project, can occur quite easily.
The first problem encountered, the circular reference, indicates a conflict in the design intent. The sleeve cannot drive the size of the hole in the plate while the hole in the plate drives the size of the groove on the sleeve. To correct this problem, the interpart links and expressions are defined in a manner so that the size of the related features, the groove and hole, are managed in a single part (the sleeve).
The second problem encountered, demonstrates the need for evaluating the effects of editing a model. A change may affect downstream features, including those in other part files. When working with WAVE and interpart expressions, it is important to think of the assembly as a whole and not merely the individual part. Also, remember that only loaded parts are updated when a change is made, so problems may not surface immediately.