How to create a WorkPoint on a SketchPoint in an assembly

[oransen]

I have an assembly.

It has a 2d sketch which contains some points.

I want to add some WorkPoints in the assembly using the sketch points (also in the assembly).

The menu to do this exists, but it does not work. The cursor does not highlight the sketchpoint, even if I push the mouse the through the tabletop.

The menu is:

    Point On Vertex Sketch Point or Mid Point.

I'm trying to avoid having a part which contains just points.

Help!

[YannickEnrico]

I don't see why that shouldn't work. That being said, why do you want the work points? I would just use the sketch points, since they have similar functionality. 

Alternatively, you can place work points at random and then constrain them. 

[SBix26]

I see the same behavior-- assembly sketch points are not available to attach assembly work points.  Not sure if that's an oversight, or as designed for a logical reason.

Sam B

Inventor Professional 2018.1.1
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[oransen]

"I don't see why that shouldn't work."

Have you tried it (in an assembly)?

"Alternatively, you can place work points at random and then constrain them."

Have you tried it (in an assembly)?

[johnsonshiue · Accepted solution]

Hi! Certainly, the behavior is not intuitive but there are technical reasons behind it. Inventor assembly (except assembly features and weldment) is not history based like part. The advantage is to allow users to structure the assembly and swap out components with ease. Work geometry is treated like a component. So, a workpoint or a workplane or a workaxis is actually a component which can be constrained to other geometry. Assembly level work geometry can be adjusted by editing the constraint values. It is not like the work geometry in a part as features.

However, assembly level sketch does have a sense of history like assembly features. Allowing non-history based operation like constraining to act on history based object can lead to an unsolvable cycle. As a result, assembly level work geometry cannot be constrained to an assembly sketch. There is room for improvement here. At least, it should be made more apparent why this operation is blocked. I will work with project team to understand the behavior better and see if the limitation can be removed.

Many thanks!

[oransen]

Thanks for the reply. I can understand the reasoning (a bit).

The menu text suggests it is possible to put a point at a sketch point, maybe that needs to be changed.

[pjvdstoel]

@johnsonshiueHave you figured something out with the project team yet? It is still in inventor 2020, and in the help. Would be nice if this was made more clear!

[johnsonshiue]

Hi! Here is an idea similar to the discussion here. Please vote for it.

https://forums.autodesk.com/t5/inventor-ideas/assembly-sketches-usable-for-constraining-and-creating...

Many thanks!

[ken.friesen]

This is not a solution. It's 2021 and still not functional

[johnsonshiue]

Hi Ken,

I never mark it a solution myself. Somebody else did. I have unmarked it now. Besides voting for the idea, there is a workflow allowing you to do that. Instead of trying to create the workpoint based on an assembly sketch point, create a skeletal part in the assembly and make it a reference. Then you can create an assembly workpoint or a part part workpoint based on the sketch point in another part.

Many thanks!

[karl.lednik · Accepted solution]

I created an empty part and grounded it at origin within my assembly.  From within that part, I created a sketch and projected the geometry I needed and constrained a sketch point.  Exit sketch and create a work point on my sketch point.  Back out to the assembly and I can now constrain to that work point.

My assembly involves a coiled part and other parts that need to be offset a certain distance from it at various points.  It's this kind of odd scenario that requires this obscure workaround.

[cmcewanE2U82]

This is still not a solution and requires an unnecessary step to create geometry within an assembly. The menu either needs to be changed or functionality added. Its now 2024...

[mark.laasu]

I just want to give a clear answer here as I struggled with it myself. This is if you wish to create a feature in assembly such as plane, axis and etc that requires a reference and you would like to sketch the reference. You can't reference a sketch that is the top (main) assembly (for reasons that johnsonshiue mentioned). Create required sketches with points and lines inside lower level (not top) part/assembly and then you can use these as a reference. If you need a reference sketch that can't be drawn in lower level part/assembly then create an empty reference part inside the assembly and sketch inside that part.

[cmcewanE2U82]

My solution is to create points delete the constraints then re-constrain the points to a plane and then constrain from the origin planes so that I can control and move the points without needing to reference other .ipt files. This would be even better if we could just do this as you would inside an .ipt with a sketch.

The limitations don't seem valid because you can still technically use parameters/dimensions from a sketch within the assembly to drive the points locations. The menu for creating points is not valid in assemblies and shouldn't tell you you can do this if its a limitation.

[mark.laasu]

I would still politely disagree with you about the "valid statement" because you can do what it says ("point on sketch point"). And when it comes to "technically possible" then I suppose it is IF you would rewrite the whole code that builds up the assembly in Inventor (probably too expensive to bother with). Reasoning behind this is that Assembly sketches can be projected from assembly parts. I think you are also able to project a work point to an assembly sketch. So if you want to sketch in assembly, add point relative to that sketch and then add another sketch that projects that point then it becomes impossible to solve because assembly is not history based. Program wouldn't know which sketch/point came first. It would be rather expensive for processor to run thru everything multiple times. Parameters and dimensions are calculated after rebuilding the model so they are not really equivalent features.
IMO it would be way simpler to create a new (reference) part in assembly, create a point at the origin of that point and you should still be able to move and constrain it as you like.

[cmcewanE2U82]

Makes sense to me when it comes to projecting. I think I was more miffed by the fact the menu says you can in an assembly and needed to come here to figure it out. I am intentionally avoiding adding more .ipt to control the assembly to reduce the amount of processing/ memory as these assemblies will be put into itables and simpler is better in my experience.

[Oliver.PearsonPV69C]

I agree. The amount of time spent trying to find what you're doing wrong because the menu suggests its possible and you can't get it to work is frustrating to say the least.

However once you've worked out that a workpoint won't snap to a sketch point (or the origin oddly), I find the quickest workaround is to choose the 'intersection of 2 lines' option then select the x and y axis, then delete the workpoint constraints and redefine them using assembly geometry, offsets from planes/surfaces etc.

[cmcewanE2U82 · Accepted solution]

My solution was adding the points to sketches in another .ipt and constraining it to the origin planes in the assembly. Seems like its an artificial limitation that can be fixed in a newer version of Inventor.