Help on Revolve, please

[NormandC]

Yes, I do want the strut to be one part. We envisage it being made from a strip stainless steel bent to shape.

Well that's important info, because it means what I was thinking of is unsuited.

Using the Sheet Metal add-on would be very relevant here, because you'd be able to easily flatten the model.

Have a look here: http://theseger.com/projects/2015/06/sh ... r-freecad/

I just tried it, and it's ridiculously easy.

FC_Maavhamt_s_sheet_metal_01.png (7.19 KiB) Viewed 1542 times

I just made a single sketch and Pad, then switched to the Sheet Metal workbench and added 2 bends. Their length has to be defined after creation, in the Data tab.

Just select a face and click on the Flatten button to get a solid flattened shape. It's not linked to the model, so if you make changes you need to delete the flattened solid and create a new one.

OS: Ubuntu 14.04.4 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6703 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 2ce5c8d2e3020d05005ed71f710e09e9aa561f40
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[Maavhamt]

Brilliant thanks I will try that. Another idea I had was to draw the profile of the strut and pad it "sideways". However I keep getting the message "Failed to validate broken face" I can't find how it is broken, do you have any ideas, please?

[bejant]

I think you used Point Onto Object Constraints where the Arcs meet the line segments. You should have selected the endpoint of, say, an inner arc and the endpoint of a line segment, then applied a Tangency Constraint to make the endpoints both coincident and tangent. After you constrain the arc centers Coincident to one another you can apply a Coincident Constraint to the endpoints of the outer arcs and corresponding line segments. Also, the blue stuff in your Sketch isn't needed.

20160727b-Strut 0.1.FCStd

(15.5 KiB) Downloaded 24 times

Edit: but by making the model this way, I don't think you can't unbend it.

OS: Ubuntu 14.04.4 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.16.6703 (Git)
Build type: None
Branch: releases/FreeCAD-0-16
Hash: 2ce5c8d2e3020d05005ed71f710e09e9aa561f40
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[NormandC]

Also, the blue stuff in your Sketch isn't needed.

+1

Not only it is unneeded, it gets in the way. I always go to great lengths not to have overlapping geometry in my sketches. I've noticed that people posting questions here along with their files add a lot of construction geometry that is redundant.

I'm not sure how you sketched your geometry, but here's a method that can be quick, and very reliable in making a valid sketch for padding.

1. Start with two rectangles crossing each other.

   

   FC_20160727_sketch_tips_01.png (3.86 KiB) Viewed 1505 times

2. Delete the upper horizontal line of the inner rectangle; use the Sketcher Trimming tool to trim the vertical lines of the inner "U" shape. You get the following closed profile.

   

   FC_20160727_sketch_tips_02.png (4.2 KiB) Viewed 1505 times

3. Start the Sketcher Fillet tool and click on the 4 bottom points of the profile. This will give you the following result:

   

   FC_20160727_sketch_tips_03.png (4.8 KiB) Viewed 1505 times

4. At each corner, select the centre point of the inner and outer arcs, and add a coincident constraint. This ensures that the inner and outer arcs are concentric.

   

   FC_20160727_sketch_tips_04.png (4.3 KiB) Viewed 1505 times

5. Add an equality constraint between the left and right outer arcs. It can be the inner arcs too, but just one or the other. If the outer arcs are set to an equal radius, you do not need to set an equality constraint for the inner arcs; being concentric to the outer arcs, they automatically adopt the right radius.

   

   FC_20160727_sketch_tips_05.png (18.89 KiB) Viewed 1505 times

You now have a closed profile of the desired shape, requiring few constraints to fully constrain it. And you can be sure that you will not get "failed to validate broken face" errors working that way, because all the geometric constraints that link elements together are added automatically by the system.

[NormandC]

Edit: but by making the model this way, I don't think you can't unbend it.

Actually you can! I just tested it on your model, and it works. But not before fixing the missing tangency condition at the top of the sketch.

FC_20160727b-Strut-01.png (19.09 KiB) Viewed 1495 times

Black circles show the missing tangent constraints. With those applied, both dimensional constraints that are crossed black become redundant.

[bejant]

Thanks again - guess I should have tried that myself...

[Maavhamt]

OK thanks I tried both suggestions and they worked really well. I think I've got a lot to learn! Really appreciate all the help from you guys.

Maavhamt.