Pitfalls of constraint creation

andrew_troup

In Part Studios

Topic 1: Constraining to entities on a perpendicular plane

Quiz Question:

Can you use a Concentric constraint, to make the endpoint of a (vertical) line on the Front plane concentric to a circular edge on (say) the Top plane?

(For instance, you might be trying to sketch the axis of an existing hole)

If not, why not?
(An error message may appear to be no help)

Follow up question:

If your answer was no, which other constraint CAN be used to achieve this result?
(Directly, between the two entities)
And most importantly, why?

shashank_aarya

My answer is no because I feel that ideally to achieve concentric constrain, two entities should be in parallel plane. Here in this case circular edge is on top plane and line is drawn on front plane, hence planes are perpendicular and concentric constrain is not accepted.
As an example we can consider two cylinders which needs to be concentric. It is easier to align them concentric when they are placed on two parallel planes, but it would be difficult when they are placed on two perpendicular planes as it requires additional tilting of one of the cylinder at 90 degree. So, I feel this can be the concept behind it.
As an alternative we can project the circular edge in front plane, create midpoint on projected line and after that end point of axis and midpoint can be constrained by either coincident or concentric constrain. Here I feel that concentric creates confusion as the term "Concentric" relates mainly to circular geometries.

matthew_menard

If the planes are perpendicular as you postulate, wouldn't a midpoint constraint work?  It seems that entities are projected from their source planes onto the working one, so a circle that is perpendicular to your current plane should be a line. 

After poking around for a minute, this appears to be true.


Center line is constrained with a midpoint, right one is coincident with the center point and the left line invokes the error message at the top.  I might venture to say that the coincident to the midpoint of the circle/arc would be a better constraint.  Only because of the off chance that your circle gets pierced and is no longer a circle, I would imagine the midpoint constraint would move where the coincident one would not.  If I have time for more play this morning, I will try and see of this is true.

andrew_troup

@shashank_aarya is, I think, exactly right.

What I'm trying to highlight here (because it is sometimes not well understood even by experienced modellers) is that constraints to remote entities are (except for "pierce") ALWAYS made to the projection of the remote entity onto the sketch plane.

@matthew_menard's post (assuming when he writes "coincident to the midpoint", he really means centre point) is also factually correct, but does not quite reflect the scenario I posted.

I was referring to a circular edge, such as the edge of a hole through a solid body, not to a sketched circle.
The distinction is significant because there is no way of inferring the centre of a hole (whereas there is, with a sketched circle)

Of course, an extra step could be added to sketch that circle, provided the hole emerged onto a planar face normal to the hole axis: the edge could be projected as a circle onto a sketch on that face, with "Use"

Because Onshape does not currently support either temporary axes (created by the software at the axis of cylindrical or conical faces) or User-specified axes, the question of how to create such constraints is, I think, a pertinent topic for serious modelling.

For instance, a workaround for their absence is to create a sketch line on a suitable plane, which will require a constraint as described above. If a suitable plane does not already exist, we have to consider how to create one, but that's another topic.

matthew_menard

You are correct that I said midpoint but meant to say center point.

Interesting though.   I was expecting to be able to "wake up" the edge of a circular cut in a model and allow it to let me snap to its center point but I see that isn't the case.  It isn't even an OnShape only issue, as the exact same behavior can be seen in Solidworks.  I'm guessing that I have never run into this problem because I've had axis available as tools in Solidworks when something like this comes up. 

It would seem that you have laid out the best work around to this given the current tools.  However, like you also said, it could potentially get messy if you are working on an axis that is randomly aligned in space that has no planer ends.

andrew_troup

@matthew_menard

Thanks for your confirmation and observations. 
Interesting point about why this deficiency is not so apparent in Solidworks - makes sense.

And your closing paragraph nails where the current capability leaves the user somewhat stranded. 

There is an IR for user-specified axes available for voting, but I'm not sure I've seen one for temporary axes.

They're a two-edged sword in Solidworks: I'm sure a better implementation could be achieved, perhaps by "waking them up" only on demand, and perhaps a one-click option to convert them to a permanent (nameable) axis.