Hi all
I have a sketch (attached) with 10 components which according to Sketcher is fully constrained - the 10 components are linked by a separate backbone in another material. But when I go to pad, I only see one of the components - and padding doesn't seem to do anything to that!
I can go into the Part workbench and extrude it; however, this doesn't appear to export an STL file that I can 3D print, whereas pad does.
I've tried this several ways, and the results always seem to be the same.
Can someone point to what's going on?
Thanks, Edwin
OS: Linux Mint 17.3 Rosa
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13522 (Git) AppImage
Build type: None
Branch: releases/FreeCAD-0-17
Hash: 3bb5ff4e70c0c526f2d9dd69b1004155b2f527f2
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/Australia (en_AU)
SOLVED: Why can't I pad this?
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SOLVED: Why can't I pad this?
- Attachments
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- RevGelas.fcstd
- (13.37 KiB) Downloaded 30 times
Last edited by earthcare on Thu Sep 06, 2018 10:31 pm, edited 1 time in total.
Re: Why can't I pad this?
Part Design creates a single connected solid. Your sketch would result in ten unconnected solids.
I removed your sketch from the body container (and deleted everything but the sketch). Deleted the redundant constraints as suggested by sketcher (this may be version specific, 0.18 adds advanced recognition of redundant constraints)
I then used the Part WB Extrude (Part WB has no single solid restriction)
OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.14570 (Git)
Build type: Release
Branch: master
Hash: 233ed49b23ee14a9978a0aa78c67396115b1582c
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)
EDIT:
Not in this model, if you had one Part Design should work. See https://www.freecadweb.org/wiki/PartDesign_ShapeBinderthe 10 components are linked by a separate backbone in another material
Last edited by sgrogan on Thu Sep 06, 2018 1:50 am, edited 1 time in total.
"fight the good fight"
Re: Why can't I pad this?
A part design body may only contain a single contiguous solid, your's produces ten!
You might consider using a part container with separate bodies within.
Steve.
You might consider using a part container with separate bodies within.
Steve.
- HarryGeier
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Re: Why can't I pad this?
Assuming this is not a technical object, but rather some sort of ART.. i would say, PART DESIGN is not the proper tool. Draft / Sketcher and Part will fit better as already posted by sgrogan
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- HarryGeier
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Re: Why can't I pad this?
Select the objects to export, go into MESH DESIGN Workbench and create mesh(ses) from Shapes. Then export them with right mouse click on the model tree, that should work for any 3D Object.
One of my videos shows a STL rework, there you can see the workflow.
here i created 3 shapes in draft, extruded in PART and converted to STL ( as you can see in the wireframes triangulated ) . After this, you can combine them to one mesh in mesh workbench before exporting, if that is wanted or needed.
- Attachments
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- 2018-09-06 08_11_56-FreeCAD 0.18.png (50.05 KiB) Viewed 1143 times
Kaum macht man´s richtig , gehts´s
My Video Tutorials on Youtube: https://www.youtube.com/channel/UCoe3B ... p8Q/videos
My FreeCAD Stuff on Hidrive: https://my.hidrive.com/share/qr3l1yddy6#$/
My Video Tutorials on Youtube: https://www.youtube.com/channel/UCoe3B ... p8Q/videos
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Re: Why can't I pad this?
Is there any advantage over the simpler way of exporting sgrogan's model directly?HarryGeier wrote: ↑Thu Sep 06, 2018 6:07 am Select the objects to export, go into MESH DESIGN Workbench and create mesh(ses) from Shapes. Then export them with right mouse click on the model tree, that should work for any 3D Object.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
- HarryGeier
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Re: Why can't I pad this?
Well,
earthcare wrote he cannot save HIS PART extrusion based model. Sgrogan´s model is PART DESIGN based approach, which might work when saved as STL .
Back in 0.16 and early 0.17 times i had a lot of trouble with STL´s created in the direct saving way ( mostly non manifold ) , so i prefer the way through mesh Workbench anyway. In addition one can check, split, combine meshes with the MESH Workbench . You can create several STL´s from a model which would probably not print well due to the positions of the solids and re-arrange them in the slicer for better prints.
As usual.. there are several ways to do the same thing in FreeCAD.
earthcare wrote he cannot save HIS PART extrusion based model. Sgrogan´s model is PART DESIGN based approach, which might work when saved as STL .
Back in 0.16 and early 0.17 times i had a lot of trouble with STL´s created in the direct saving way ( mostly non manifold ) , so i prefer the way through mesh Workbench anyway. In addition one can check, split, combine meshes with the MESH Workbench . You can create several STL´s from a model which would probably not print well due to the positions of the solids and re-arrange them in the slicer for better prints.
As usual.. there are several ways to do the same thing in FreeCAD.
Kaum macht man´s richtig , gehts´s
My Video Tutorials on Youtube: https://www.youtube.com/channel/UCoe3B ... p8Q/videos
My FreeCAD Stuff on Hidrive: https://my.hidrive.com/share/qr3l1yddy6#$/
My Video Tutorials on Youtube: https://www.youtube.com/channel/UCoe3B ... p8Q/videos
My FreeCAD Stuff on Hidrive: https://my.hidrive.com/share/qr3l1yddy6#$/
Re: Why can't I pad this?
Harry, thanks for the info. Especially the fine tuning possibilities might be useful.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
Re: SOLVED: Why can't I pad this?
Hi all
And thanks to sgrogan - I got it to work with your approach.
And thanks to sgrogan - I got it to work with your approach.