Sheet Metal Workbench

[thebighaggis]

Hi easyw-fc

That's just what I've been looking for..thank you very much... I'll have a look at this tomorrow...8pm in Australia time for a beer

Again thanks...

Cheers
Haggis...

[thebighaggis]

Hi easyw-fc
I had a look at the spreadsheet option for adding
Custom Kfactors and this works well, I also added another spreadsheet so the foldwall calculations are correct when flattering the blank again eg 100x100x2mm square folded through the middle with foldwall tool never flattens out to 100mm it's smaller... that's using the standard Kfactors eg 0.33 to 0.5 range..
I had to fudge the Kfactor to 0.16 to 0.18 to get it close.."I know it's nowhere near any Kfactor range but it works as long as the inside radius = material thickness...
I have these tables created and named them material_std and material_foldwall...so depending on what method I use I can set to the correct one...
I usually use standard tools to create sheet metal parts but sometimes my customers have only the flattened blank and require a 3d drawing that must be accurate when folded up..whew....almost there
My question is how do I set this up so when I start a new part the spreadsheets are there..as it is now I have to copy and paste from one part to another...
Sorry for the long post but I just wanted to explain why it was so important to me to get a correct 3d finished folded part using the foldwall tool and fudging the Kfactor...
Really appreciate your help here..

Cheers.
Haggis

PPS
I understand how it works now... I thought the Value in the 1st cell was the material thickness, is see now I was wrong..
So basically I would need to make spreadsheets for all my material types... eg
For common bends default inside radius = material thickness so in the table it would be set to 1.00 in 1st column..
material_MS ( Mild Steel) using 0.41 as Kfactor and inside radius same as thickness but for larger radii use 0.5 Kfactor
material_SS ( Stainless Steel) using 0.38 as Kfactor and inside radius same as thickness but for larger radii use 0.5 Kfactor
material_AL ( Aluminium) using 0.52 as Kfactor and inside radius same as thickness but for larger radii use 0.5 Kfactor
Then for anything 3mm and over 0.5 Kfactor.. ( so just use default Manual Kfactor )

Is that correct?

I would still would like to know how to have this setup so when i start a new file the spreadsheets load automatically

[PeterPNoster]

Hello thebighaggis
I have similar issues with sheet metal.
My approach is:

• Build up a 'customer deduction table'

• So I check every sheet metal and do some bending test at different bending angles.

• The results go into a Python script

• The resulting formula values are used to calculate all other deduction values at the relevant bending angles

The result is something like that.

deduction.png (53.29 KiB) Viewed 2395 times

A drawback is, I have to do this for many different material, tool, bending direction and die combinations.
But I suppose once set up, the consistency between design and bending results, should be much better than with any other method.

An other plus is, that the 'real' values can be used in e.g. Trumpf Boost software, once 'Kundenverkürzungswerte' will work properly...

A long-term goal could be, to put the functionality into FC sheet metal wb. As an alternative to the k-factor thing. So a possible plan could be to have the possibility to use real measured deduction values if available, or go the k-factor way.

[jaisejames]

Some big fix on size calculation issues. Pls update & test it to latest version. Pls give feedback.

[thebighaggis]

Thanks for the post PeterPNoster

Hi Jaisejames

Excellent work on the fold wall tool, absolutely brilliant very happy
I did a comparison with AutoDesk Inventor & FC Sheet Metal WB
Material 2.0mm
Flat blank 100x100
Added 2 sketches 25mm in from ends to create channel
Set inside radii to 2mm
Set Kfactor to 0.41
And the results are Identical , it also flattens back out to 100mm
What can I say... great work..

This is the only thing I've tried for now, if you have documentation or youtube
video on additional tools in Ver 2.4 could you please share and I'll test them
too..

OS: Windows 10 (10.0)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.20996 (Git)
Build type: Release
Branch: master
Hash: 9b8b128a0d9990da44f7a2f00c9dc9ae152a5985
Python version: 3.6.8
Qt version: 5.12.1
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/Australia (en_AU)

Cheers
Haggis

[jaisejames]

Three new commands added to convert solid to sheetmetal. Relief, Junction, Bend

Step 1.
Create a thin solid like this.

solid.png (30.3 KiB) Viewed 2227 times

step 2
Then create relief on corners by selecting corners & select relief command.
Adjust parameter to get cut more than inner radius

Relief.png (25.18 KiB) Viewed 2227 times

Step3
Then create Junction by selecting edges.
Adjust parameters.

Junction.png (28.42 KiB) Viewed 2227 times

Step4
Then create bend by selecting edges.
Adjust parameter.
Note : bend can be added after fully open-able/unfold shape only

bend.png (35.99 KiB) Viewed 2227 times

Unfold it.

unfold.png (30.53 KiB) Viewed 2227 times

[chrisb]

Thanks! To select a corner it is just the vertex?

[shaise]

Thanks! To select a corner it is just the vertex?

Yes, a single vertex. Great job, jaisejames!

[drmacro]

When I attempt bend it fails. I'm guessing it's my settings for thickness and radius...but, changing doesn't seem to help. Shown is the default1mm radius, 1mm thick.

Sheetmetal_corner.png (81.67 KiB) Viewed 2186 times

[Kunda1]

can someone make a short gif of the new commands, pls ?