Multi-Body Cut

[Anonymous]

I have created a feature (v-groove) that cuts through two bodies (veneer and core).  When using the rectangular pattern option to pattern the first v-groove,  the groove does not cut through both bodies.  No method of selecting the additional body seems to work.  Any help would be appreciated.

[swalton]

Check the compute options in the feature pattern tool.  You might need to change from Identical (the default) to Adjust.  Hit the >> button to expand the tool and check the options.  See my screenshot from IV 2014.

If that is not it, try using the Solid selection tool to get both solid bodies. (under the feature selection tool)

[fakeru · Accepted solution]

I think Inventor doesn't allow you to cut material with pattern feature from more than one solid.

The fact that it says "Solid" and not "Solids", probably is an indication of that.

What I use to do in this case is simply make another pattern future for the other body. I link the parameters between the two pattern features, so when I make changes in the first one, the second is also updated.

[swalton]

@fakeru

I don't use mulitbody solids much, so good catch.  I like your workflow.

Another idea, model as a single body solid and then use the split command with a parting datum or surface to separate into the substrate solid and the veneer solid after all the common features. 

[blair · Accepted solution]

It only allows for a single solid to be selected for the Pattern. No wonder I'm not a big Multi-Body Solid user.

[SBix26]

As others have noted, this is not currently possible.  I have submitted a proposal to the Inventor IdeaStation to correct this "defect".  Please add kudos to this idea: Pattern/Mirror Features in Multiple Solids.

Sam B

Inventor Professional 2015 SP1 Update 1
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M