Derive Flat Pattern of Part

[emanuel.c]

Thought to ask this: Is it possible to derive into a new part the flat pattern of another?

Reasons: Edits on flat pattern which would be used for CAM (machining) programing.

Thanks!

[kacper.suchomski]

Hi

I do not know what you mean. You can, for example:

1. Use a flat pattern in InventorCAM
2. Use the Unfold tool and create a Model State that you will insert into another file/program.

[Gabriel_Watson]

Right-click the Flat Pattern node in the Inventor browser > Save Copy As > select SAT (.sat) as format under "Save as type" > import it back into a new part in Inventor to add your edits.

SAT works similarly to STP.

[emanuel.c]

Yes, @kacper.suchomski it totally needs more explanation. So what happens is, say we have a flat pattern of a part which needs machining. Perhaps the outer profile is enlarged for this pupose, or some holes are filled in "smaller" for latter machining / removal of material. So when laser cutting I edit the flat pattern to add material where needed.

For programing I need both the "stock" profile and the "finished" profile of part. Unfortunately, in CAM I have to have 2 separate bodies for specifying first the "stock" part and then the "finished part" - model states won't do.

This is my current workflow. In the part to be machined I Thicken/Offset or Direct Edit the profiles which need machining (to what they will be cut - what is set in the flat pattern). Then I create a copy of the body as new surface and suppress the Thickened surface. Now in CAM I can select as stock the copied body and select the solid body as finished part (model body).

It can get tedious considering many, many parts. Also because of suppressing the Thickened surface and copying body, those links are disconnected, so updates to the part will not apply.

@Gabriel_Watson Yes I suppose that is a workable solution, save for the fact there will be no dynamic updates... No more links to the original part, in case of updates.

Does this make sense? Is there a better workflow that you all can suggest? I was thinking to create a new part in which I derive once the flat pattern and secondly the finished model, in order to have these 2 bodies to work with.

Many thanks!

[kacper.suchomski]

I thought of two strategies:

1. Working with model states:
   1. Create a new model state
   2. Create operations: Unfold, Thicken, Refold
   3. Disable these operations in one of the model states
      
      This way you will get a model with two states, one of which has the areas thickened by the allowance.
      
      
2. Derived component
   1. Create a nominal plate
   2. Derive part
   3. Convert derived part to sheet metal
   4. Add allowance (in model or flat pattern mode)

[johnsonshiue]

Hi! Or, you may export the flat pattern as STEP. Then associatively import it to a new ipt file. When there is a change in the flat pattern, just export it again (overwrite the existing STEP file) and the linked Inventor part will update accordingly.

Many thanks!

[Frederick_Law]

Does the CAM need 2 bodies?

Or it can be 2 files?

I used Model State for "finished" punch flat and a "purchased blank".

[CCarreiras]

@Frederick_Law , CAM needs two bodies (Multisolid): One body to select as stock and the other is the part itself.

CAM will not import the flat pattern, so the only way i see is to unfold the model.
If you want to have associativity with the source file, i would go for the derive method, which @kacper.suchomski refered, then, unfold the part and create the extra operations.

[emanuel.c]

@kacper.suchomski,  Thank you for your thoughts. I'll have to play around with this. I like the idea of using the different model states, versus importing .SAT or .STEP. The only issue is to mind another program we use for nesting (ProNest) which doesn't work well with Model States: it may totally skip parts which are not being used with the "Primary" Model State in an assembly.

@johnsonshiue,  It would be really nice if CAM could use Model States for this purpose. It seems to me, this is one of the reasons it's designed for. Only one part to reflect both states.

Thank you.