falviani wrote: ↑
Fri Sep 04, 2020 3:31 pm
drmacro - I'm afraid it's unclear to me how to restrict my references to another sketch when editing. I hope to find that out from the video tutorials. I often find the 'copy' tool in the part design workbench won't work with the sketch I want to copy in for reference, for reasons I don't understand.
I know of no 'copy' tool in PD workbench.
That doesn't mean there isn't one though...
In any case, the way to reference geometry from other sketches needs some explanation that you my not find in tutorials, or may not recognize it when you see it.
- Select the PD workbench, start a new file.
- Create a sketch (it will create a Body for you and the sketch (Sketch) for you on the plane you selected.
- Draw rectangle. Close Sketch.
- Create another sketch on the same plane, it will be named Sketch001.
- Draw a pentagon or some shape other than the one in Sketch. Don't close this sketch.
- now click the Model tab (you are probably in the Tasks tab)
- The first Sketch is gray-ed out. Click on it and hit the space bar. ( You should now see the geometry of Sketch and Sketch001)
- Now click tis icon:
and hover your mouse over a piece of geometry from Sketch. If you click it will produce a pink line matching the Sketch geometry.
- You can now constrain Sketch001 geometry to the pink line.
Having done that if you now close Sketch001 and open Sketch and change it's length, Sketch001 will update with it.
This is also sometimes called the Master Sketch technique, since you may never pad Sketch.
( Also, with the sketches close, select Sketch001 in the model tree. Look at the properties. Expand the Attachment group and change the Z value. You'll note the sketch moves up the global Z axis.)
There are other techniques as well, spreadsheets, dynamic data, links, shape binders...
In general, do you have any hints as to what caused the main plate sketch to shift when I changed the sketches for the additive loft? I find that mysterious.
When the topo naming issue causes loss of reference the solver can do some seemingly very strange things. That'd be my first inkling...
I still have 2 questions about log/report messages:
1) "PartDesign::AdditiveLoft / AdditiveLoft: Links go out of the allowed scope". Hopefully rebuilding the model will alleviate this - but what is the 'allowed scope'?
2) "SketchObject::onChanged(): Unmanaged change of Constraint Property results in invalid constraint indices" - this is completely obscure. Is this due to sketches that are not completely constrained?
#1 usually happens when you create and reference a sketch that was created outside the Body (i.e. the property value Map Mode is "Deactivated" and Support is blank, typically because the Sketch workbench was used to create the sketch and not the create sketch in Part Design.
#2 typically this indicates the constraint it is complaining about no longer has the face or edge it was referencing. I.e. the topo naming issue.