Lesson Objective: In this lesson, we will learn how to create exploded states, complete with offset lines.

















Text Box: Assembly
Mode – 
Assembly Cuts



There are a variety of reasons to create cuts in the context of an assembly.  The most common are:

·            Cut-Away Views – You create a cut that removes volume from some or all of the components in the assembly.  Unlike a cross-section, which will remove volume from all of the components when you set the visibility to view the cut-away, an assembly cut allows you to selectively pick which components are affected.

·            Holes/Cuts in Weldments – Adding a hole pattern or cut to an assembly that represents a single weldment.  The ability to create the holes in the individual parts is minimized, because of dimensional references that may or may not exist.




We will work with the stacker assembly that we created in Lesson 38 to demonstrate cut-away views.  Open up this assembly, and it will look like the following.



We want to make a cut that removes half of the volume from all of the components except the stem part.  Before we do this, however, let us look at a cross-section for this part.


To do this, go to View, View Manager.  When the view manager opens, click on the Xsec tab.  Create a new cross-section called Cut_Away, and use the ASSY_RIGHT datum plane as our reference (pick it from the model tree).


Once you have created this cross-section, double-click on it.  We see the following.



As you can see, the cross-section view removes half of the stem as well as the rest of the components.  We want to see the entire stem.


Therefore, we will use an assembly cut.  First, close out of the view manager, and go into the layer tool.  Hide all _Defaults layers except for the assembly itself.  Your assembly should look like the following with datum planes visible.



Now, click on the Extrude tool.  Down in the dashboard, you will notice that the “Remove Material” icon is grayed out.  The reason for this is that any solid feature created in assembly mode can only remove material, not add material.



Now, click on the Placement slide-up panel.  It looks like the following.



We can either select a sketch feature in the assembly, or create a sketch.  We will click on the Define button.  For a sketching plane, select the ASSY_TOP datum plane, and face the ASSY_RIGHT plane towards the Right.


Inside the sketch, select the outermost circle (both halves) as sketching references.  Then, sketch the following rectangle.  Be sure to impose a tangent condition with the side, and snap to the top and bottom of the circle.


Finish out of the sketch, and make sure you go to the Options slide-up panel and select Through All for both directions, as shown below.



Finally, go to the Intersect slide-up panel.  It looks like the following.


By default, all components in the path of the cut are going to be listed in the window.  In this case, all seven parts are listed.  We will start by un-checking the Automatic Update option at the top.  This allows us to selectively add/remove models from the list.  We will scroll to find the STEM model, and right click on it.  Select Remove from the list of options, as shown in the next figure.


Click on the green check mark to finish this extrude feature, and we will be left with the following.


The Stem part is completely unaffected by this cut.  The other models are only cut away in the assembly.  If you open the Base or any of the rings, they still are whole.  We will show something different in the next section.  To turn off the cut-away, either delete the extrude feature or suppress it.


Save and close this assembly.  We will come back to it in the last lesson.








The other common usage for assembly cuts would be in an instance where you can not easily define a hole or cut in a single part that may affect a group of parts.  A good example might be a welded frame that will get items mounted to it.  The spacing of the holes, as well as the locating dimension for the holes is usually determined after the frame is completely welded.  But, for manufacturing reasons, we need to model the members of the frame separately and use an assembly to define the overall frame.


Change working directories over to the Weldment folder, and open the assembly entitled Welded_Frame.asm.  It looks like the following.



If we expand the model tree, we can see the product structure as follows:



The overall frame (gray bars) is welded together.  The plate on the side (green) will be bolted onto the frame.  In order to ensure that our bolt holes line up perfectly, we could do a number of things.  Perhaps the cleanest would be to develop a skeleton for the interface points, and develop the weldment and the plate from this information.


In this case, we are working with existing assemblies, so we only have two choices.  We can go into each model, create separate holes/cuts and then build in relations between components to determine the location in case a change is made.  This is a perfectly acceptable way of doing it, but creates a lot of book keeping.  It also assumes that each hole can be manufactured off of existing references in the part file.  In our assembly, we want to locate the holes from the extreme ends of the assembly, so it won’t work at the part level without adding extra datum planes or surfaces to capture the envelope of the assembly.


Therefore, we will create the cut at the assembly level, and then discuss how we might be able to transfer that information into the parts (if required).


Creating the Cut


Click on the Extrude tool once more.  Define the sketch, and use the front of the plate as a sketching plane, and point the ASSY_RIGHT datum plane towards the left.  In sketch mode, change your display to a hidden line mode.  If your sketch doesn’t automatically pick references, select ASSY_RIGHT and ASSY_TOP for sketching references.


Zoom in on the upper left corner, and sketch the following:



Now, pan over to the upper right corner and sketch two more circles – making sure to align the centers where applicable, and dimensioning where necessary.



In the lower right corner, sketch two more circles, as follows:



Finally, in the lower left corner, finish sketching the last two circles, as shown.  NOTE: You shouldn’t need any dimensions for these holes, as the centers should line up with existing circles or references.



Zooming out, our entire sketch should look like the following.



Finish out of the sketch.  For a depth option, pick on the To Select icon (the one with the red), and pick the following surface.



Now, we will click on the Intersect slide-up panel.  It currently looks like the following.



We can see four MAIN_BAR models listed.  In reality, the holes that we are creating are not going to intersect these models, so we will remove them.  To do this, un-check the Automatic Update option, and then right click on each of these bars to remove them.


We are left with two SIDE_BAR, two MID_BAR, and one SIDE_PLATE components, as shown in the next figure.



One other thing we can see in this window is that each component has a value of Top Level, in the Display column.  This means that the cut will only show up in the top-level assembly where it is created.  We will right-click on each of these models in the list and change the option to Part Level.  The intersect window will look like the following when we do this.



Click on the green check mark to complete this extrude feature, and you will see the following on your model.

From this figure, we can clearly see holes on all of the mid and side bars.  The reason for this is the cut has been translated into the actual part file.  If we open the SIDE_BAR component, for example, we see the holes.



In the model tree, it indicates the Assembly Cuts, as shown in the following figure.



If you try to edit or edit the definition of these features in the part itself, you will find that you can not.  You have to go back to the assembly to edit them.  This is intended functionality.


If we had kept the models at the Top Level scope, this is what we would have seen at the assembly level.

We can see that the holes are only on the side with the plate.  All other Side and Mid bars are unaffected.  If we open up the same SIDE_BAR model, we don’t see the holes, and the model tree does not list the assembly cut features.



The advantage of placing the visibility of the holes at the part level is that we can detail out the part in drawing mode and dimension the holes accordingly to perform the drilling at the part level.  Of course, if this had been the original intention, we might have wanted to just create them as part cuts, and then tie them together with relations at the assembly level.


The disadvantage of placing the visibility of the holes at the part level is that the model being cut will now have the holes in every instance that is used in the assembly, as we saw in our model.  The work-around to this would be to model completely different bars for the side with the plate than what is on the rest of the frame.  This creates more models than we really need.  Of course, had we needed to add a plate to the other side, we can now just assemble in one more with the bolts and nuts and we won’t have to necessarily cut additional holes out.




Assembly cuts are great for creating cut-away views that can’t be done with cross-sections, or for creating cuts/holes in an assembly and showing the visibility at the part level.


Be sure to look at the list of models that the cut will intersect, and remove any models that you don’t need in the list.




Open up the model entitled Shelf.asm.  It will initially look like the following.



For this exercise, we need to drill holes to screw the pieces together.  The following figures show the locations for the holes.  We also need these holes to appear at the part level to be able to detail out the individual boards.