Maintaining material thickness in the bend radius

[jcook27FELS3]

I watched an excellent YouTube video from John H. on bending parts which helped me design the bend for my aluminum bracket parts, however the design is not maintaining the bend radius or material thickness I expected. I believe this has something to do with the bend options: corner relief, override rules or bend relief override - but I haven't got this figured out.

Hoping you can help. I want to maintain the aluminum material's thickness of 1.5 mm and the inner radius should maintain that 1.5 mm in the bend.

Attached are two bracket types. Thanks.

- John

[kacper.suchomski]

Hi

In the bending dialog box, you have the option to override the bend radius value checked and a manual value entered.

Uncheck these options to keep the nominal value from the sheet metal rule.

[jhackney1972 · Accepted solution]

I have attached your model with your requirements.  If you need explanation, please ask.

[laughingcreek]

you have a bunch of extra and unnecessary steps in your process that are probably confusion you. see attached.

note 1-when you use the bend tool, the bend created is defined in the bend tool, not in the Sheetmetal rule.

note 2-usually you would model the part in the bent form, and use the unben tool to create any features that need to be worked out in the unbent form.  the bend tool is really for a different workflow.

note 3 - you didn't have your bend line position defined.  this seems like it would be an important dimension. if you want to use the bend tool, you will have to manually calculate where it needs to be.  or you could model it in the bent form and let fusion do the heavy lifting. 

EDIT:  was the sketch imported?  in that case using the bend tool this way is appropriate.  it's primary used for re-creating Sheetmetal parts from existing flat patterns that are imported. 

[jcook27FELS3]

The override was selected to try and maintain the thickness. Without it selected the thickness is 2.0 mm. So I was trying a bunch of different settings.

[jcook27FELS3]

Hi John

I followed these steps from your YouTube video for bending using the sheet metal tools.

After I imported my dxf file and extruded to 1.5 mm, I did the following:

01. Create Sketch on backside
02. Project command for the whole outline with Projection link ON
03. Finish Sketch
04. Go to Home position
05. Go to Sheet Metal menu
06. Create Flange
07. Pick the sheet metal side to have thickness go up into the part
08. Select metal type and click OK
09. Make another sketch on the sheet metal surface (backside)
10. Draw bend line(s) and click Ok
11. Go to an Isometric view
12. Turn off solid body and just deal with metal flange
13. Under Sheet Metal menu select Bend
14. Choose the stationary side
15. Choose the bend line
16. Choose any needed bend override and click OK
17. Turn OFF sketch view
18. Turn Solid Body view back ON
19. Go to Sheet Metal menu Modify / Unfold
20. Select Stationary surface
21. Select Bend surface(s) and click OK
22. Merge sheet metal part into body using Solid Menu Combine option
23. Target body = Sheet Metal Body (pick it from the browser)
24. Tool Body will be the Solid Body (pick it from the browser)
25. Click OK
26. Go to Sheet Metal menu and select refold

If you could elaborate I what I was missing or did wrong I would appreciate it. I'm going to be doing a lot of bending...

Thanks!

John

[jcook27FELS3]

Yes, the dxf file was initially imported into the sketch.

The specific steps for bending my part was using a sheet metal technique I saw in John H's video. If there are other ways to bend - I'd like to learn those as well.

John

[kacper.suchomski]

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@jcook27FELS3 wrote:

The override was selected to try and maintain the thickness. Without it selected the thickness is 2.0 mm. So I was trying a bunch of different settings.

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Global values ​​should be set in the Sheet Metal Rule, not in the parameters of individual operations.

If you create a rule, you won't need to change, overwrite, or search for anything.

Furthermore, the sheet metal base plate should be created using the Flange command, not the Extrude command. This way, all values ​​will be automated and synchronized.

[jhackney1972]

A lot of good comments and suggestions have been made by other users, be sure to read them.  I went through the creation of one bracket just to illustrate that you really did a lot of unnecessary work to create your bracket from your DXF.  Also, it is very important where you place your bend line and be sure to constrain it in place with a dimension.  When using the Bend command, it is important to calculate the location to get the correct bend position.  I cannot over emphasis to get your Sheet Metal Rule established before doing any modeling, it governs most operations in the sheet metal environment.  The creation of a sheet metal component was good but the creation of extra components was unnecessary.