Hello all
I “suspect” that the command Solidify or Cut is not behaving in well in an assembly containing pattern inside Creo / Creo simulate. So far there is no explicit restriction when using it.
As we know solidify/cut is very useful to explore symmetry in FEM to reduce computing time. Especially in Creo solidify is a good approach if your model contains components having volumes regions to be used inside the simulation. From my experience it is easy to “lose” these volumes made in the CAD parts when you have an assembly that was cut using extrude/revolve feature – but this is another case…
The below assembly (4 CAD parts) was also made patterning some sub-components.
When I try to simplify it using the feature "solidify" (fig. a) the result is bad. If instead I create a volume to cut half of the assembly (fig. b) the result looks god – but not once the model is inside Cre Simulate (fig. c, d)!
a
b 
c
d 
I do not see any logic or restriction why these commands should not work well with pattern. One can argue that since the model contains pattern we can pattern just enough to create the symmetry. This is indeed what I think I have to do in this case but truly it is not the best way since you have to build the model again – what can be very time demand in some cases.
_Has someone faced such problem and found a solution or work around?? I´m using Creo 2.0 M150.
Thanks,
R. Rabe
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Thanks Kevin
But I´m sorry to say that I could not understand how your explanation can be applied in the assembled case. Or is it basically a comment?
Just to make sure I just picked-up a datum plane of my choice and applied the command found under ”Modifiers>Solidify” in the assembly model.
From my understanding it simples “cut” the entire assemble to the left or right depending of the choice.
The problem is that or it behaves completely erratic or there are some important rules to follow – that I really don´t know.
For example here is the assembly model “fe_asm0_v2” that you can find in the message from Paul (above). I have just added two new datum planes.
I created a diagonal plane in the height direction and the solidify result was ok in CAD and inside Simulate.
Now I just created an offset plane in the side direction. The result is bad and also completely different depending even the direction of the cut!
Indeed the best solution is to prepare the symmetric model since the beginning (a suitable CAD parts design) and not after, using cut-extrude or solidify function in the final assembly.
"Cut" and "Pattern" have relationship problems when sharing the same assembly...
In order for a solidify feature to remove material the feature used to cut the model has to meet certain conditions it doesn't just simply remove what's to the left or right of the plane. In the case of a cutting plane (datum plane) the plane must intersect (pass through) the feature geometry or model geometry.
In your second picture it's a bit hard to tell what the cutting plane passes through but it looks like it passes through all the parts (pieces). In the third picture the orange wedges in the center, the outer ring, one of the inner grey rings, and two of the wedges between the cylinders have material removed because the cutting plane passes through the geometry, the cutting plane doesn't pass through any of the cylinders. In the fourth picture the same parts (pieces) have the opposite side of the material removed because you changed the side of material removal.
You can see the same behavior in a part. You see it by having the plane pass through the solid geometry, when you move the plane in the direction opposite to the direction the direction arrow for material removal points you should see more of the geometry gets removed from display. When the plane no longer intersects the geometry the entire part gets displayed.
You also see this behavior in a part if geometry regions are not connected. If the plane passes through only one of them, the region the plane passes through will have material removed the other will always display.
I'm not a Simulate user but from the steps I've seen used to prepare models I could see where an assembly cut might cause problems if my assumptions are correct. My assumption is Simulate would want the cut at the part level. Since you are using a pattern of a part you run into problems since you have a part in three states: no removal, partial removal, and complete removal of material. My guess, based on on what I'm seeing, is your original assembly with the hub, outer ring, cylinders and retainers would only end up with the hub and outer ring if the intersected cut was redefined to intersect at the part level.
