Bending dimensions for press brake

[Anonymous]

Hello, 

I am using Inventor and me and my company never used it before. since it is one of my first sheet metal component I am creating , I am facing few issues. The models I created have several bends. These components are laser cutted and therefore manufactured on a press brake. I need to know the dimension to input on the press brake so the back gauge stops on the right place. The first bend is not difficult, because I can see the dimension from edge to the bend center on the flatt pattern. the second bend needs a dimension from the flange of the first bend to the bend line of the second bend for a back guage setting. However, I cant see this dimension. I have searched other similar posts but I couldn´t understand it very well:http://forums.autodesk.com/t5/inventor-general-discussion/dimensions-for-press-brake/td-p/4383084

I am able to see the the press brake back gauge distance for 1, but not for 2 

Any help is welcome, Thanks

[Anonymous]

Anyone can help me? I just want to know how can I take these dimensions out of Inventor.

[swalton · Accepted solution]

Inventor does not have an easy button for what you want, but you can get there.

You can use a combination of the ipart workflow and the Unfold feature to create additional part models, based on your finished model, that show the different stages of forming the part. 

See http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-DD9F389B-4B23-482A-A46E-4CA71101658A for IV 2014 iPart info.

Try this:

1. Model your part in the finished shape.  Make sure you use the correct k-factor for your press, tooling, material, and operators.

2. Add unfold features to your ipart to show the forming steps.

3. Convert your sheetmetal part to an iPart.  This becomes the iPart Factory file that defines all the possible variants of the part.

4. Edit the iPart table and create a member for each of the forming steps by suppressing/enabling the unfold features as required.

5. Make sure to create a member that shows the finished component too.

6. Create your idw and make your first base view show the fully-formed member.

7. Add views as required to show the forming stages of the part. Select the correct iPart Member for each stage.

8. Dimension views as required.

9. Use the fully-formed iPart Member in any assemblies that use this part.  If you used the iPart Factory file from Step 1 in an assembly, you need to change it to the fully-formed member created in step 5.  Constraints will break, so be careful.

[Anonymous]

Thanks, I will try follow those steps and see the result

[Anonymous]

Here is one article writing about sheet metal parts bending, including the method to calculate the calculation of sheet expansion length, it will help you.

https://machinemfg.com/parts-bend-forming-technical-study/

[Anonymous]

It's been three years...

One should hope he's found a solution by now. 

On topic, we use software that came with the pressbrake to do the actual calculations. We design in Inventor sheet metal as desired, then export the .stp. Really the only way to go imho, as bend forces, bend losses etc. also depend on the materials used, not just the thickness of the sheet.

[Anonymous]

Bend allowance, bend deduction, K factor, unfold length is what you should take into consideration. You can use the Fabrication Calculator to get the above data before bend.