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Spit one part into two

ptc-968028
1-Newbie

Spit one part into two

Is it possible to take a single solid part, cut and separate along a datum plane, and have 2 parts? I do alot of fixture design concepts where I work out geometry and feasibility in several large complex parts in an assembly. When it comes time to detail for manufacturing, alot of the complex solids need to be made from multiple blocks, but when assembled retain the same overall geometry. I have been creating new parts and cutting down the old ones, but it would be much easier if there were a way to just cut the solids into multiple parts. Does a function even exist to do such a thing in Pro/E?
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4 REPLIES 4

I suggest you make a family table to create your parts from the generic. Two cuts can be created off the datum plane in opposite directions. Suppress the cuts after each is made in the generic part, and in the family table add both cuts as feature columns. The generic row will show N indicating the features are suppressed, while the instance rows will have an asterisk (*) indicating the generic default. Change the cut appropriate for an instance from * to Y (unsuppressing it for that particular instance) and from * to N for the other instance(s). Verify and preview the instances.

I'm not sure I understand your needs precisely, but two points: 1. Douglas' technique will work as stated, and can also be accomplished without a Family Table. If you were dividing one part into three with two parallel planes for example, you could create necessary cut features in the Master Model, suppress all of the cuts, copy the model three times, then resume the different cuts as necessary in the copies. 2. You mentioned fixturing. If you are creating a fixture with multiple blocks, then nesting something complex into these blocks, you can assemble "uncut" blocks, then cut them all within the assembly using the complex reference geometry.

There are all sorts of ways you can do this easily, but without seeing the parts its hard to walk you through it. You can try emailing me a sample part.

click the datum plane, click EDIT-> SOLDIFT. Select material removal and one side is done. you also can create two such features, one for each side and add it to family table. Keep in mind that, it better to ceate one, add it to FT, supress that feature and then go to the next. HTH. Joe. ---------------------------------------------- you can find some tips at... http://tipsfromjoe.blogspot.com ---------------------------------------------- .
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