Use Cabling for boolean subtraction?

[DevinHahne]

Sometimes it's helpful to be able to subtract a Creo Cabling assembly from solid geometry.  Article - CS36069 indicates the way to do that is by exporting an IGES file of the cable and then re-importing that into Creo Parametric.  It's not ideal, but it at least provides a way of doing this subtraction.

Is there a way to directly reference the cabling geometry, as a Copy Geometry or Shrinkwrap feature, in a solid part and perform this boolean subtraction?  Ideally the solid part would be able to reference the Cabling assembly directly, to maintain parametric relationships.  Is the IGES export method the only option?

[Chris3]

I don't know if you are aware, but Creo doesn't model cables as solid geometry. Cables are curves with surfaces. For this reason you can't use Boolean operations with them.

I haven't tried this myself, but I believe you should be able to set the curve as a publish geometry feature and then in your next assembly use that curve and sweep along it with a cut feature. This isn't exactly what you were looking for but is slightly more parametric then the IGES method.

[DevinHahne]

Hi @Chris3,

Thanks for your response!  Yeah, all my reading and experience so far concludes cables are not solid.  I tried using external copy geometry features to pull the Network segments into other parts, but the segments were not selectable.  Actually, it would be more useful for our process if we could ECG the curves rather than the cables themselves.  But so far, it's no good.  The best thing we've been able to do is to place datum points on the Network segments and then run a datum curve through the points.  Then that datum curve can be ECG'd into other parts.  Not an ideal solution because it requires maintaining those points (e.g. if segments get deleted).  And this process would be unrealistic for large Cabling assemblies.

[Chris3 · Accepted solution]

ok I just tried out my proposed solution myself and it works, but it is not robust at all.

I created an assembly with a harness in it and I created a point to point wire in the harness. Then I created a new part and used the copy geometry feature to pull in that curve feature. I referenced the assembly model, turned off the published geometry only button and then selected the chain group and used the find tool to find 3D curves with sub models. All of this worked and now I had the cable spline in my new part file.

I then added a location in my harness to change the curve. I went back into my new part and did a regen and the copy geometry feature failed because the curve was now 2 curves and it lost the reference to the original curve. So it worked, but it is not very robust. Once it was 2 curves I updated my intermediate location feature and that did update without failures. So if the cable geometry fairly firm and all that is going to change is small cable location movements then this might work but probably not great for early design work.

[DevinHahne]

Oh interesting!  I didn't think to try using the Find tool in the Chain references collector.  I'll have to give that a try.  And thanks for the warnings!  I'll follow up on this thread soon.

[DevinHahne]

I finally got to test this technique and found that it works!  The challenge I had with using the Find tool was making sure "Look for" was set to "3D Curve", History tab was set to "All", and then "Look in" was set to the Cabling part specifically.  That let me select the Network curve segments.  One additional challenge is, it wants to grab all the cable segments as well.  So the user attempting to create the ECG will have to be careful to select only the Network segments.  Thanks again @Chris3!