Offline Programming of Amada Press Brakes

[CadManagerMoffatNZ]

Good morning Inventor Community

This post doesn't directly relate to any deficiencies in Inventor but is aimed more towards its integration into a modern manufacturing environment, but that said it could be a good case for the Autodesk Manufacturing guru's to look at 😉 as not all of us use 3D Printers and Generative Design to manufacture parts.

A little background on this subject.

We use Inventor to design our product lines and historically we would create a dxf for laser cutting / turret punching of the sheet metal components and a fully dimensioned idw showing a flat pattern with bend lines and the projected orthographic views with the critical / overall finished sizes shown. The guys on the press brakes would then use a hard copy of the idw to write the programs for the press brakes. This system has worked and been refined since we began using inventor 5.3. Accuracy of finished folded parts within 0.1mm.

Fast forward to 2018.

With out getting into the full and messy background, we (and that's the royal "management we") implemented offline programming of the press brakes utilizing Amada SheetWorks.

This has and is not going well.

To get a folded part that is anything like accurate we are now having to compromise the ipt's and the way we model them. (I'm happy to share the actual details in a DM if required).

Does anyone have experience of using Amada Sheetworks in a full production environment with Inventor?

And or what else is being used in the community to take Inventor sheet metal components thru the manufacturing process.

Current Workflow.

Inventor 2019 creating ipt.

Inventor 2019 creating a 3 basic view "Design Intent" drawing of the folded part with overall finished dims.

Ipt exported to STEP format.

STEP imported into Amada Sheetworks.

DXF created for laser / turrets.

Shop floor drawing of the flat pattern (used in the press shop to identify the blank) overall x & y dims only.

MBF (Model bend files) created for the 3 variations of Press Brakes.

Either DM me or post here if you wish

Thanks

[kitchenqueen]

I was just wondering if you ever got any help with this. Sorry to bother you 10 months later

[timDS75C]

Would love to hear how you are getting on with any of this, "We" recently got a new Amada press brake with the said sheetworks software, now i'm having to do the same process.

I also use Solidworks and the Sheetworks software actually pulls the actual Solidworks model files instead of having to convert to anything else. 
We have spoken to Amada who say they are still working on updating the software to support inventor, anything before 2019 inventor isn't supported. 

[CadManagerMoffatNZ]

Hi Tim

Yes I have managed to solve the issue for us and i have to say the automation that Sheetworks offers is showing itself to be worth the pain.

Step 1.

Re-write our bend tables.

This was achieved by reverse engineering sample folded sections of each and every gauge / type / finish of material. Measuring actual bend radii and calculating k-factor and bend deductions. Very time consuming but vitally important that this is "perfect" as best you can measure.

Step 2.

Update the materials and bend tables in Sheetworks.

Step 3.

Update the sheet metal styles in Inventor to use the new bend tables.

And here is the big trick that i only discovered after much hair loss and trial and error.

Because (as you have pointed out) Sheetworks will not accept native inventor files we export *.stp files that Sheetworks then imports and "re-builds" with Solidworks features etc the Inventor *.ipt must be very clean before export. By "clean" i mean no corner treatments, nothing can modify the bend plates in any way.

In the image below i have highlighted this. The red arrow shows our "old" Inventor standard corner detail, the green arrow show the new standard.

Bend plate

With clean *.stp files Sheetworks will create Bend programs without error. If the stp contains any bend plate modification Sheetworks will fail to create a bend program with minute line replacement errors. 

Step 4.

Flat patterns modification.

We don't use Sheetworks for the flat pattern generation. The x & y overalls will match the inventor flat pattern exactly because of the effort put into the "shared" bend tables but Sheetworks puts "random" corner replacement cuts into it.

So we add the correct (accepted company standard) corner replacements into the flat pattern before exporting a dxf for nesting. 

This has 2 advantages for us.

1 It allows the designers to control the correct overlaps for downstream processes (welding and or consumer interaction).

2 The programmers (Sheetworks users) don't have to second guess the design intent and check that Sheetworks has applied corner replacements correctly.

Here is a real world part based on the above routines ready for laser welding. 0.9 AISI430 Stainless steel.

Hopefully this small little tips we get you going in the right direction.

On a good day Sheetworks and the ATC Press Brakes are the best things.

I can design a new part and within 30 minutes i can be fitting on one of our products. (Inventor - Sheetworks - Laser nest & folding solution - to me.)

The accuracy of offline programming is +/- 0.1mm on finished sizes virtually unheard of from our manual programming days.

Let me know how you get on.

[timDS75C]

Thank you very much for such a detailed write up.
Although you may have just created me a lot of work XD, At least now we can get on the right track maybe. 

[davew]

We use Radbend which is quite good. It will take the inventor model as designed including the Flatt pattern size