I'm trying to align some propellers to a drone model. I have 4 propellers to align. I managed to get plane alignment working fine but axial alignment has only been successful on one of the props. Please could someone have a quick look and tell me where I'm going wrong?
The 3 problem alignments are "AxialAlignment001" to "AxialAlignment003".
I am using the latest git Assembly 3.
Many thanks.
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 2021.1015.24301 +3962 (Git) AppImage
Build type: Release
Branch: LinkStage3
Hash: c6cb39697eb439caf7e5bd0208ca3082a7820547
Python version: 3.9.7
Qt version: 5.12.9
Coin version: 4.0.1
OCC version: 7.5.2
Locale: English/United Kingdom (en_GB)
Assembly 3 Axial Alignment Failure
Forum rules
Be nice to others! Respect the FreeCAD code of conduct!
Be nice to others! Respect the FreeCAD code of conduct!
-
- Posts: 169
- Joined: Sat Jan 23, 2021 1:15 pm
Re: Assembly 3 Axial Alignment Failure
This is common problem with Assembly 3: the solver will fail if parts are overconstrained.
You used Plane Alignment that fixes X, Y rotations and Z translation and Axial Alignment that fixes X, Y rotations and X, Y translations. That means X and Y rotations are constrained twice.
Quick and dirty fix: disable plane alignments and recompute. Parts will move in X and Y axes. Then enable plane alignments and recompute second time. Parts should move to their final positions.
Better fix if you have two circular faces on your both parts: use Plane Coincident instead of two constraints above.
Better fix if you do not have circular faces or do not want use them: add a point in one part and axis and second one and then use PointOnLine constraints plus Plane Alignment constraint.
You used Plane Alignment that fixes X, Y rotations and Z translation and Axial Alignment that fixes X, Y rotations and X, Y translations. That means X and Y rotations are constrained twice.
Quick and dirty fix: disable plane alignments and recompute. Parts will move in X and Y axes. Then enable plane alignments and recompute second time. Parts should move to their final positions.
Better fix if you have two circular faces on your both parts: use Plane Coincident instead of two constraints above.
Better fix if you do not have circular faces or do not want use them: add a point in one part and axis and second one and then use PointOnLine constraints plus Plane Alignment constraint.
-
- Posts: 169
- Joined: Sat Jan 23, 2021 1:15 pm
Re: Assembly 3 Axial Alignment Failure
Okay, well I hope Realthunder can fix it. I just donated to help him.
Okay, that will do for me. I understand this as I come from Solvespace where this was the only way to mate parts together.
Thanks for your help.
-
- Posts: 169
- Joined: Sat Jan 23, 2021 1:15 pm
Re: Assembly 3 Axial Alignment Failure
Okay, posting again as I couldn't make it work. I added a point constraint on the sketch of the rectangle of the prop (Body_Prop -> Pad_Blades -> Sketch) which is used for padding but in the Assembly 3 workbench, that point does not appear. Where am I going wrong?kwahoo wrote: ↑Fri Nov 12, 2021 2:57 pm This is common problem with Assembly 3: the solver will fail if parts are overconstrained.
You used Plane Alignment that fixes X, Y rotations and Z translation and Axial Alignment that fixes X, Y rotations and X, Y translations. That means X and Y rotations are constrained twice.
Quick and dirty fix: disable plane alignments and recompute. Parts will move in X and Y axes. Then enable plane alignments and recompute second time. Parts should move to their final positions.
Better fix if you have two circular faces on your both parts: use Plane Coincident instead of two constraints above.
Better fix if you do not have circular faces or do not want use them: add a point in one part and axis and second one and then use PointOnLine constraints plus Plane Alignment constraint.
Thanks again.
Re: Assembly 3 Axial Alignment Failure
FreeCAD does not show points from a sketch outside the sketch. You can create a second sketch with a line (or lines) and end of the line will be selectable as a point.
Or you can use datum point https://wiki.freecadweb.org/PartDesign_Point
- adrianinsaval
- Veteran
- Posts: 5541
- Joined: Thu Apr 05, 2018 5:15 pm
Re: Assembly 3 Axial Alignment Failure
You can have a defining point in FreeCAD since 0.19
https://wiki.freecadweb.org/Sketcher_Cr ... nt#Options
By default points are created as construction geometry and therefore are not visible outside of Sketch editing mode. Use the Sketcher ToggleConstruction.svg Toggle Construction tool to change them to normal geometry.
Re: Assembly 3 Axial Alignment Failure
It doesn't "need to appear" - with sketch visible, and desired entity (point etc) selected, you will see in tree view sketch selected - drag it to create element to use with assembly constraint.exsolvespacer wrote: ↑Fri Nov 12, 2021 5:07 pm ... I added a point constraint on the sketch of the rectangle of the prop (Body_Prop -> Pad_Blades -> Sketch) which is used for padding but in the Assembly 3 workbench, that point does not appear. Where am I going wrong?
In the pic below I have selected a point in the sketch (made visible), and you can see sketch selected to the right- just right click drag it to elements:
-
- Posts: 169
- Joined: Sat Jan 23, 2021 1:15 pm
Re: Assembly 3 Axial Alignment Failure
Thanks a lot. I had no idea you could do that (and perhaps others didn't too).bambuko wrote: ↑Sun Nov 14, 2021 9:56 am
It doesn't "need to appear" - with sketch visible, and desired entity (point etc) selected, you will see in tree view sketch selected - drag it to create element to use with assembly constraint.
In the pic below I have selected a point in the sketch (made visible), and you can see sketch selected to the right- just right click drag it to elements: