Sheet Metal Design?

[jmaustpc]

I don't think this is much help but just in case...Once I modelled a thin plate duct using a sweep. You can set the corners of the sweep path to rounded or you can actually define the curve within the path itself. In this example I used a path without defining the curvature of the joint and then used the "rounded corner" transform from Part Sweep.

In this drawing you can adjust the angle constraint from 90 to 180. This only works on one plane, so it could make a duct but not a box.

sheetmetalducting2-folded_and_unfolded.fcstd

(22.7 KiB) Downloaded 791 times

If you search this forum for "sheetmetal workbench" you will find where we have talked about this in the past...might be worth a read...if you haven't already.

The previous work on a fold/sheetmetal workbench was never actually a part of FreeCAD itself...it was a extension someone wrote that you could download from another site. I don't think it did much or got very far ...but I could be wrong...also I have no idea if it would still work or not...anyway I thought there might be something useful for you in the code ....so here is is.

fold_v1.zip

(526.08 KiB) Downloaded 418 times

I wish you well with this, it would be a great addition to FreeCAD.

Jim

[calgarykev]

Great, thanks Jim!

We will have a look at your zip file. I will have to do some reading on the "sheet metal" search of the forums.

Kev

[jmaustpc]

Great, thanks Jim!

We will have a look at your zip file. I will have to do some reading on the "sheet metal" search of the forums.

Kev

Just to be clear, I did not write that code..I just downloaded it from the author.

Jim

[NormandC]

Hello Kev,

I've been designing sheet metal parts (produced by air bending, or to those not familiar with the name, using a press brake - wiki link) for a long time. I used to work with AutoCAD which had no flattening capability, so I had to draw flattened parts manually. For the past few years I've been working with Solid Edge which has a complete sheet metal module with flattening capability, this is a huge time saver! And less error-prone.

I don't code so I can't help with that, but I'll sure be willing to test what you come up with.

Thanks Mark! This is a starting point. It's a surface so no thickness. If you come across any examples involving solids, I would sure appreciate a link.

That's the hat trick isn't it... calculating the material consumed in the bend and adding it to the length, on the proper side of the break, when the part is unfolded.

Actually, working with surfaces might be sufficient and something like that unfolding macro could be used I think.

Mark, nice find on the video, it's a good explanation. I think a good bet is going with the K-factor. For example, assuming a K-factor of 0.33, you offset the inner surfaces of your sheet metal part by 0.33 X the sheet thickness. This will give a set of surfaces placed on the neutral axis. You then unfold these surfaces to get your flattened part.

I was able to do this with the GUI tools, so I guess it would be possible to automate this. Since the goal is to project the flat in a drawing view, and maybe export it to DXF for laser cutting, I don't think it would be really useful to generate a solid.

FC_sheet_metal_flattening.png (20.1 KiB) Viewed 9659 times

At my old job, I took our bending tables and using a spreadsheet I came up with K-factor values for all materials we were using. With those values the flattened parts were very precise.

[calgarykev]

Actually, this brings up one of the complications of doing sheet metal with parametric solids. I have been using AutoPol with my Mechanical Desktop and they don't generate a solid of the flat. They just give a 2D flat in paper space that sometimes updates to changes successfully but often fails. This big problem with this method is that dimensions on the flat are non-associative to the drawing and must be manually rechecked/repositioned every update.

The benefit of the solid should be associative dimensions that update with the changes. However, this means that we must tie/link our individual flat features to a corresponding bend features on the original part. Hence, we update it if the original changes or eliminate it if the original feature disappears. Again we need to learn to mine the solid for meta data so we can get each feature's "serial number" so we know what to do: create, update or eliminate.

Then end goal is to have a flat that updates as long as the base feature is in tact. To have dimensions associate, it may be possible without a solid, we may be able to link them to the 2D rep; we need to investigate that. In some ways, this would be superior as there is less clutter to manage in the real 3D assembly. We need to see what can do with the kernel functions and make a decision on this.

Kev

[scons]

+1 for developing a Sheet metal Workbench

I think the bending factor (K-factor) should be accesible in 2 ways:

• - a "general table" for calculations
  - a customizable table for calulations

Why ? The thicker the sheet is, the higher deviations will be. For example: a sheet of 2mm bendend over 90° will give a different length then a plate of 15mm ...
Also the bend itself needs to be considered. For example a bend over 45° will give not to very little deviation, but a bend of 135° will give a lot ....
Some people will have different bending equiptment and get different results, so they should be able to customize the tabel for their needs.

So let's take a sheet from 0-2mm (S235JR aka metal):

TH = stands for the actual thickness of the sheet in the equation

Degrees - Deduction Mass - Bending Radius

45.0 - 0.0 - 2.0*TH
90.0 - 0.1*TH - 1.6*TH
135.0 - 0.2*TH - 1.2*TH
180.0 - TH - 0.5*TH

When you take this to a plate of 20mm you get things like:

45.0 - 0.0 - 1.2*TH
90.0 - 0.5*TH - 1.0*TH
....

The above does not apply to aluminium or other.

These are reasonable settings to start from for calculations i think.

[jmaustpc]

Hi scons
Sounds like something that might be able to utilise a spreadsheet workbench. Someone was working on a C++ implementation to replace the current Python one.

Jim

[cblt2l]

I do a lot of goofy transitions in SW. Normally I make a solid loft and then use the 'Convert to Sheet Metal' tool. You select the face of the solid that represents the fixed face of the sheet metal part and then select the edges of the solid that correspond to the bends. Its a nice way to make complicated shapes without having to do a lot of trial and error.

The 'Apply a Thickness' feature in the Part workbench is very similar, except that the process is reversed (i.e. you select the faces that get removed rather than the faces that stay). Maybe it could be expanded further into a sheet metal tool .....

[jmaustpc]

I don't have time to experiment just now ... however check this out.

If you make a 2d face you can apply the Part "Offset" tool and click "create solid".

So if it works the way I think it does ...the edges will be normal to the plane at that point, so if the plane is bent through 90degress then I think the two edges would generate correctly, at 90 degrees to each other.

[dode]

Also +1 for this. I'm a newbie with freecad but been flattening sheet metal with 3d cad and without for 25 years. The best reference is DIN 6935 for bending and I think that was here the k-factors started. If you need any practical help I can share experience and talk through the approach typically used in doing this stuff manually. I did write some macros originally in APT (yep that olde) later in various 2D or 2 and a bit D packages to create flat patterns of standard items.

George