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constrain 2 circles

dlaery

Alibre Super User
how do I constrain the 2 sketch circles?
I have tried concentric and coradial and i get error on both "over-constained or inconsistent sketch"
i want the 2 sketch circle to stay together when I drag or constrain to something else.
 

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Ken226

Senior Member
I tried recreating your sketches from the image you provided, and am having no problem getting the constraints to work.

Can you upload the file your having trouble with. Perhaps the way you sketched them resulted in some automatically applied constraints that are restricting movement.
 

HaroldL

Alibre Super User
Did you sketch the two circles one on top of the other? There may be an inferred constraint involved. Also in the image it looks like three circles are highlighted. Could that be confusing the constraint system?
 

dlaery

Alibre Super User
thanks, i tried a new part and it worked. the problem I seem to have is when designing something using sketches and make changes I run into lots of trouble with sketches, not being able to find the over-constrained part. so in frustration I start over and sometimes it works and sometimes I go a completely different direction
I was having trouble drawing the dark green part. I wanted to make a snap piece to go on 1/2" pvc.
instead of circles i used arcs and offset.
 

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Ken226

Senior Member
thanks, i tried a new part and it worked. the problem I seem to have is when designing something using sketches and make changes I run into lots of trouble with sketches, not being able to find the over-constrained part. so in frustration I start over and sometimes it works and sometimes I go a completely different direction
I was having trouble drawing the dark green part. I wanted to make a snap piece to go on 1/2" pvc.
instead of circles i used arcs and offset.

Holding the Ctrl key while dragging sketch parts should temporarily allow you to override the inferred constraints and move the sketch figures.
 

dlaery

Alibre Super User
Did you sketch the two circles one on top of the other? There may be an inferred constraint involved. Also in the image it looks like three circles are highlighted. Could that be confusing the constraint system?
yes, well the 3rd circle should not have been highlighted. in the attached file I was trying to do reversed arcs to make the snap, I thought 2 circles, use the tangent then trim what I didn't want, seemed simple to do until it was over-constrained, then it is like I can't do anything, so i gave up and tried plan B, but I did want to know how to constrain 2 circles, so when i tried the new part, it worked like I thought it should, but I certainly agree with your question "Could that be confusing the constraint system?"
 

Ken226

Senior Member
Your assembly had some overconstrained issues.

I changed the planar constraint you used to lock the support, to a free offset. I constrained the free offset horizonatal reference plane to the assemblies default plane and that cleared up all the red/error constraints.

1659467987421.png
 

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Ken226

Senior Member
I recreated the problem you were having, and it was driving me nuts not being able to figure out why I couldn't get the concentric constraints to work.

I did manage to figure out though that when you un-lock the horizontal reference line, the concentric constraints start working normally again!

@HaroldL

Why does using the lock constraint on an unrelated reference figure kill my ability to constrain the circles concentric to each other? Is that normal?



After I deleted the lock constraint on the horizontal reference line I was able to constrain the two circles concentric to each other. Then I reapplied the lock constraint on the horizontal line. It appears to work fine that way. It just won't allow the circles to be constrained while that reference line has the lock constraint applied.
 
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HaroldL

Alibre Super User
Why does using the lock constraint on an unrelated reference figure kill my ability to constrain the circles concentric to each other? Is that normal?
That sounds like a question for Alibre Support or Development. Unless there is an inferred constraint between the circle and the line. :confused:
 

HaroldL

Alibre Super User
I was trying to do reversed arcs to make the snap,
David, have you though of using the Thin Extrude? You won't have such a complex sketch if you do, I've worked one out with three tangent arcs.

1659497977089.png

Because Thin Extrude in on the drop down menu I kind of forget it's there. Although I have been trying to use it more lately for simpler parts since it simplifies the sketch.
 

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dlaery

Alibre Super User
thanks, i don't think things very far ahead sometimes, so when I started to draw this, I use "Project a Sketch" a lot so that is how i started with the 1 circle and then offest the thickness, then I thought I would draw the 2 circles, constrain them and move over to the other 2 circls until the tangent attached, but anyway I'll try to remember the Thin Extrude, I forget it is there alsol
thanks,
 

jfleming

Senior Member
It could all be made a lot simpler if there was just a list of the sketch constraints that exist, those which were inferred during sketch creation, and the ones applied by the user. The inferred constraints are tough to deal with, especially if you didn't know they were created when you drew the sketch.
 

dlaery

Alibre Super User
I thought his would stop the inferred constraints but I can tell any difference by have all of these off.
 

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Max

Administrator
Staff member
thanks, i tried a new part and it worked. the problem I seem to have is when designing something using sketches and make changes I run into lots of trouble with sketches, not being able to find the over-constrained part. so in frustration I start over and sometimes it works and sometimes I go a completely different direction
I was having trouble drawing the dark green part. I wanted to make a snap piece to go on 1/2" pvc.
instead of circles i used arcs and offset.

If you begin the node of a circle (or any sketch figure) on the node of another sketch figure, the nodes are locked together (through an inferred Coincident constraint). Since we don't want dozens of coincident constraints to litter the canvas for every node pair, we don't show those. However, if you construct the circle like this, the centerpoints are already coincident. I think in the circle node case, the Concentric constraint is what actually gets made first, instead of the coincident constraint.

What you may have also done is drag and drop the circle's centerpoint node (or any node of any figure) on top of another node (in this case the 2nd circle's centerpoint) and it will make a hidden coincident constraint.

Since this hidden coincident constraint already exists, making the circles concentric will overdefine them since they are already concentric. Since you have dimensions, especially different dimensions, on the circles, a co-radial constraint does not make sense. CoRadial is typically mode useful for arcs.
 

dlaery

Alibre Super User
If you begin the node of a circle (or any sketch figure) on the node of another sketch figure, the nodes are locked together (through an inferred Coincident constraint). Since we don't want dozens of coincident constraints to litter the canvas for every node pair, we don't show those. However, if you construct the circle like this, the centerpoints are already coincident. I think in the circle node case, the Concentric constraint is what actually gets made first, instead of the coincident constraint.

What you may have also done is drag and drop the circle's centerpoint node (or any node of any figure) on top of another node (in this case the 2nd circle's centerpoint) and it will make a hidden coincident constraint.

Since this hidden coincident constraint already exists, making the circles concentric will overdefine them since they are already concentric. Since you have dimensions, especially different dimensions, on the circles, a co-radial constraint does not make sense. CoRadial is typically mode useful for ar
ok, thanks. I opened a new part sketched a circle at .85 and created another circle, selected the centerpoint to create a circle at 1.05. select the center and drag both wherever I want. I opened the file I was having trouble with and did the exact same thing on an existing sketch (the pkg file is uploaded to the thread) and the attached pic shows the result of trying to drag. I just couldn't figure out what I was doing wrong. also I have the inferred constraints all un-checked and always have, not sure if that makes a difference. I am just trying to learn here.
thanks,
 

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