Hello. I have a helix and a sketch profile for the thread I want to cut from a part-design body. I don't really care what bench I use, as long as at the end I have a body with a shape that I can change with less than 3 steps if I need to redesign the threading. I remember using a similar procedure and getting success, but when I select the sketch I want to sweep, and then the helix, FreeCAD doesn't throw any error in the console, it simple fails to create a solid.
I have tried both the Part and Part Design Tool benches. The threading is Garden Hose Thread, btw.
Any ideas? Thanks for any help.
Female thread cut profile & helix; Part bench will not create solid
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Female thread cut profile & helix; Part bench will not create solid
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- femal_ght_to_half_hose.FCStd
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Re: Female thread cut profile & helix; Part bench will not create solid
Install ThreadProfile workbench, tools menu -> addon manager -> workbenches
Make Body active, right click -> toggle active body.
Create new vthread profile. Select ThreadProfile object in properties view select MapMode property, click [...] button to bring attachment editor. Select circle edge shown:
Select ThreadProfile, in properties -> V Thread presets -> Garden hose NHR thread
Set Internal/External property to Internal
Set Height property to 14 mm
Select ThreadProfile object, execute Make Helix command. This makes a new helix of appropriate pitch and attaches it to the thread profile object. Note the Helix faces the wrong direction, so toggle the ThreadProfile MapReversed property to True.
Select both the Helix and the ThreadProfile object and with both selected execute the sweep command.
Make Body active, right click -> toggle active body.
Create new vthread profile. Select ThreadProfile object in properties view select MapMode property, click [...] button to bring attachment editor. Select circle edge shown:
Select ThreadProfile, in properties -> V Thread presets -> Garden hose NHR thread
Set Internal/External property to Internal
Set Height property to 14 mm
Select ThreadProfile object, execute Make Helix command. This makes a new helix of appropriate pitch and attaches it to the thread profile object. Note the Helix faces the wrong direction, so toggle the ThreadProfile MapReversed property to True.
Select both the Helix and the ThreadProfile object and with both selected execute the sweep command.
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Re: Female thread cut profile & helix; Part bench will not create solid
Thank you TheMarkster. This workbench looks like exactly what I want to make threads in the future. Unfortunately it seems to be pretty glitchy (Cannot change diameter of helix and pitch isn't calculating threads per length correctly from height value), but I will try to install the latest version of FreeCAD and see if that makes everything go smoothly.TheMarkster wrote: ↑Tue Nov 30, 2021 3:56 am Select ThreadProfile, in properties -> V Thread presets -> Garden hose NHR thread
Set Internal/External property to Internal
Set Height property to 14 mm
Re: Female thread cut profile & helix; Part bench will not create solid
I admit I didn't study this too hard, so I may be completely missing the issue.
And, @TheMarkster's recommendation is perfectly ok as well.
But, works for me once the sketch is put in the body and a Part Design workbench Subtractive helix is used with the parameters used in the Part workbench helix...
(FreeCAD file is too big with the threads modelled.)
And, @TheMarkster's recommendation is perfectly ok as well.
But, works for me once the sketch is put in the body and a Part Design workbench Subtractive helix is used with the parameters used in the Part workbench helix...
(FreeCAD file is too big with the threads modelled.)
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
- Shalmeneser
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Re: Female thread cut profile & helix; Part bench will not create solid
Reworking everything, no TNP.
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- femal_ght_to_half_hose_SHALM.FCStd
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Re: Female thread cut profile & helix; Part bench will not create solid
The helix should not set directly, but instead through properties of the threadprofile object. I don't think the helix diameter matters the way the workbench uses it.WhisperingShiba wrote: ↑Tue Nov 30, 2021 7:11 pm
Thank you TheMarkster. This workbench looks like exactly what I want to make threads in the future. Unfortunately it seems to be pretty glitchy (Cannot change diameter of helix and pitch isn't calculating threads per length correctly from height value), but I will try to install the latest version of FreeCAD and see if that makes everything go smoothly.
There does appear to be a bug in the Height to Thread Count conversion. As a workaround, I think if you set Height to something else and then back again it will calculate correctly. I'll see if I can figure out what the issue is.
Edit: I pushed an update that hopefully fixes the issue. If you don't mind testing it I would appreciate it.