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Modeling Finish Stock (Cutting prior to machining)

We cut a lot of parts from plate that get turned in a lathe or otherwise machined. Is there an easy way create in a model, and on the subsequent drawing, the finish stock required? We pull parts studio parts directly from OnShape directly in to our nesting software so I need a modeled part I can nest. Take a look at the shared file, it's a couple simple flanges. I've modeled the (2) flanges. Then I modeled a third part to represent my burn-outs as shown on sheet2 of the drawing. My visual preference on the drawing is a phantom line representing the burn-out or material to be removed but of course still need something I can pull into Sigmanest.  What I'm doing works but seems cumbersome. I wondering if there's an easier way.

https://cad.onshape.com/documents/8f3480dc07fd47ed307aef0c/w/2cb077e97aa3d803a522b57d/e/7a969ca11d8162f85138e469

Thanks in advance for any thoughts/advise,
Kent

Best Answer

Answers

  • mahirmahir Member, Developers Posts: 1,018 ✭✭✭✭
    You could create separate configurations for different machine operations.
  • mahirmahir Member, Developers Posts: 1,018 ✭✭✭✭
    Here's a link to your same part but with configurations applied. Keep in mind most of your drawing views/dimensions would need to be recreated since the parts are now really the same part instead of the different parts.

    https://cad.onshape.com/documents/72e167d4f62ee42caae9fafd/w/4bac3a02de6537f931d939c6/e/91d5d8f7e3c795c06f3914ba
  • mahirmahir Member, Developers Posts: 1,018 ✭✭✭✭
    @John_P_Desilets, I ran into something odd creating the above example. If creating the blank by configuring selections on Extrude1, the part created was considered a different part. Even though all 3 configs only created 1 part, OS considered the part created by the Blank config separate from the other part created bye the C'bore and Threaded configs. This made configuring part name and appearance pretty tricky. The only way I got it to work properly was by configuring OD/ID instead of changing the selected faces to be extruded. I understand this is better practice anyway, but I still wouldn't expect an extrude to create a part with a completely different ID just because the faces selected were different. Or would I?
  • ilya_baranilya_baran Onshape Employees, Developers, HDM Posts: 993
    Yes, the sketch entities for an initial extrusion (loft, sweep, etc.) determine the identity of the resulting part -- this is to support multi-part modeling.  One common trick is to make a big box as the first feature and then boolean intersect it with whatever you end up with -- that way the identity of the result part will be the identity of the unconfigured box.  Another possibility is we could provide a feature that explicitly names a part, giving it a new identity -- that might be more confusing, though...
    Ilya Baran \ Director, Architecture and FeatureScript \ Onshape Inc
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 3,269
    Here is one process you could try (even though I've not tried it myself):

    1. Derive finished machined part into another Part Studio
    2. Add material to the part in reverse machining order (i.e. last machined face should be first material add operation)
    3. Repeat until full blank achieved
    4. Use configurations to suppress each of those features in order
    5. Create a drawing showing each machining operation if you so desire!

  • mahirmahir Member, Developers Posts: 1,018 ✭✭✭✭
    edited February 2018
    No offsense, @NeilCooke, but that sounds hokey :P 

    @ilya_baran's method sound a little less hokey.

    It isn't a big deal though. I think it only comes up when using different profiles to generate the base feature of a part. I don't think that's a common occurrence. You can easily overbuild the part and then cut away what you don't want instead.
  • michael3424michael3424 Member Posts: 523 ✭✭✭
    I think that most, if not, all CAM provide a feature for adding stock to a part imported from CAD programs.  The one I'm familiar (SprutCAM) with is a matter of a few seconds to use.  Do any pro machinists or CAM operators see a need for what the OP is requesting?  I'm just an intermittent machinist so would freely admit that I could be missing something here.
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 3,269
    @mahir no offence taken  ;)  That was the process used by a very well known aero engine manufacturer. Who am I to argue?  :p
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