Coincident constraint always constrains a point to line - not a point to a point

[mhag33tg2]

Inventor help information here; https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-A85A7A30-7D81-4C75-8769-CAD034EEA930

says  "The Coincident constraint causes two points to be constrained together, or causes one point to lie on a curve.

".  Bold underline added.   But it does not say how to get one end point to constrain to just another end point.

I can only get a coincident constraint to constrain a point (at the end of a line) to another line so that the point can move along the line.  I can't get the point on the end of one line to constrain to the point of on the end of another line.   Not being able to do this causes all sorts of problems and limitations. 

In this mode, if for example you constrain two line ends together, of say line A and B, it is apparent that the end of A gets constrained to the whole of line B.  But also the end of line B gets constrained to the whole of line A.  This  "dual crossed" constrained seems to have the effect of pinning the point in space, with each line preventing the end point of the other line from moving anywhere.   And rather than the constrained end points acting like a pin joint, it also seems to inadvertently/unwantedly constrain the angle between the two lines

I have searched help and the forums but can't find how to do this.

Any suggestions?  Hopefully I have just missed a setting or special instruction.

BTW, I think this should be possible because Fusion sketches normally work like this, for example;

Starting shape - a rectangle with all constrains removed except coincident constraints

Distorted shape - made by dragging bottom right corner point away

[YannickEnrico]

A: Is this a scenario you cannot reproduce? Green has already been selected and red is possible to select

B: I don't see how it would constrain any angles between the lines. If you take two lines without any other contraints than a coincident constraint on end points, they're free to rotate about the constrained point, but they behave differently depending on whether you grab the pin, the line or the unconstrained end points.

[mhag33tg2]

Anyone can easily replicate this. What you say is what I expected, but that's not what it does. If you carefully constrain the green end point of one line to the green end point of the other line, being careful not to select any whole lines, then you get a yellow point at the join, and the point can no longer be moved. And if the other end of one of the lines is attached to something else then you can't drag & rotate that line either. If your Inventor functions different to mine then I'd like to find out why. Did you stick those two lines together and try it?

[YannickEnrico]

The yellow point means it's constrained, and you can hover the mouse over it to display the constraints in the point.

In regards to whether you can rotate it or not - Did you make sure absolutely all other constraints are gone? You can press F8 and F9 to toggle display of constraints

The pic below displays a Vertical constraint and Project Geometry "constraint" (in my colour scheme, projected geometry is green)

[YannickEnrico]

Inventor auto creates some constraints depending on your settings, and I suspect that's what you're encountering.

You can change those settings as shown below

Edit: If this doesn't solve your problem, maybe you can attach a part exhibiting the behaviour so I can investigate?

[Alexander_Chernikov]

This is a workprocess video.

Can you make a video of your work to see the problem?

[CCarreiras]

Hi!

Tip: You can even drag one point to another point to create the coincident constrain:
(it will work with circle centre points and middle line points)

 

[mhag33tg2]

Yes. Hovering done. Absolutely made sure all constraints are gone, except coincident ones. See pic below with F8 pressed to reveal all constraints.

A is fully constrained to the origin.

B is completely unconstrained - it would appear - but it is constrained in some ways.

C is internally constrained with right angles only, no dims, and one corner connected to one corner of box A via coincident constraint.  C cannot be freely rotated other than by the rotate command.  When command used it warns it will break some constraints but afterwards no constraints seem to be lost.

D is internally constrained, and dimensioned.  And before connected to A, it can be moved only in the direction normal to its sides, so does not rotate and has limited translation direction.  Then when connected to A at one point via coincident constraint - it can no longer be moved or rotated.  D can only be rotated by the rotate command and after that it breaks the coincident constraint. But the contraint it breaks is the one at  A1 on shape A.  And it keeps it broken, then D can be moved around but not rotated by grabbing.

Grabbing and pulling point B1 on B does not change the shape of B

B does not rotate if grabbed anywhere, and cannot be changed by grabbing a corner, such as B1.   If grabbing a line, on B the line can be moved and it stays connected to the other lines - and with constrained angles.

[mhag33tg2]

My last reply was based on these settings.

I tried it again with these settings. Same result.  Lines in boxes B C D do not rotate.

F8 shows this now. No change to constraints.

[YannickEnrico]

Can you share your model? I'd like to inspect the constraints

[YannickEnrico]

These settings only apply when you're drawing, so disabling them afterwards changes nothing - So I'd only expect a different result if you redrew

[CCarreiras]

Well, that's how it works.

At the end of the day, all the geometry must be constrained, so, why you need all that "free" moves and rotations?

What you need to achieve that you can't get it now?

[mhag33tg2]

Thanks Alexander. I tried exactly what you did. Draw two separate unconstrained lines, constraint one point to the other. Try to drag a line, it goes as yours does - all good.   Try to drag by the yellow joining point and it does not budge and angles of lines do not change.  Will see if I can do a vid.

[mhag33tg2]

I appreciate that when I eventually move on towards a physical design I will have 3D parts that can rotate and they will all be based on fully constrained sketches, but for the time being I want to work on some 2D sketches that are partially constrained, so that I can quickly experiment with geometry and movement.

[mhag33tg2]

File attached.

[YannickEnrico]

B has its end points connected - thus is behaves like earlier examples posted here. If you pull a point, the connected lines rotate. If you pull a line, it'll keep the angle and move the points.

C can be rotated if you add dimensions to it - Sorry, that's just how Inventor works. In this particular instance it'll resize the rectangle before rotating it - So if you tell it the dimensions, it'll rotate it.

D if you lock a point it'll rotate around it - But it won't behave like there's some kind of gravity or resistance affecting it - So it'll keep its rotation until you lock a point.

I'm seeing the behaviour I expect on my installation - If you can get video of it behaving differently, I would be interested to see that

[mhag33tg2]

Thanks Yannick.  Mine is not working like that.  Now you've got me thinking there is some application setting I need to adjust.  I'm now trying to remember how to do a video.  Did one a long time ago but I've forgotten how.  Not sure if i do it through Autodesk viewer or other way.  Maybe you can point me in the right direction?

[YannickEnrico]

Autodesk Screencast - Allows direct upload to your autodesk account as well, so you can post it here

Woops.. Screencast is no longer a thing as of jan. 2023... So yeah, now I'm not exactly sure what capture method would be best - OBS studio supports well compressed files so it doesn't take up too much space to capture a recording.

[kacper.suchomski]

The Inventor interface has logic such that constraints take precedence over geometry. Therefore, when you create a coincidence constraint, it always points to the constraint first. If you turn off the visibility (not operation) of constraints you can easily grab a corner of the line.

Yellow point is a coincidence constraint symbol (not a geometric point).

This works well.

[mhag33tg2 · Accepted solution]

Thanks Kacper. I can't quite see what you are doing there.  Text in menu looks to be Russian, but seems to be in same place as "Hide" for me.  OK, i see that if you do that to one of the constraints, the yellow dot disappears and then the lines move as as desired, but as soon as you click on a line the yellow dot comes back and it locks up again.   It does not seem reasonable to have to keep hiding constraints to do that.  Maybe I am confused here, but I really think it should be able to operate normally with the yellow constraint indicator showing, especially given that Autodesk says the coincident constraint can act on points and given the ends only were picked. 

Rectangle D seems to have to have two constraints at one point hidden to un-obscure the vertex and allow box D to rotate.  Then you have to grab only that vertex and nothing else.  If you accidentally click a line connected to that hidden constraint then the yellow dot reappears and then if you try to grab and move the vertex, the thing wont rotate.  The method can work but its clunky and unintuitive.   

Are you in effect saying that the yellow dot that indicates the constraint existence is getting in the way of the actual intersection point and preventing me from selecting the actual  intersection point?  Even if that was the case, if constrained box D for example was not constrained from rotating, like mine, shouldn't you be able to grab it any where to rotate it?  And especially so if the yellow marker obscures the vertex grab point.  It would make more sense if you could leave the yellow dot showing and just grab any line to make a constrained shape rotate?  Fusion works like that so it is doable.

Your advice is a good step forward towards resolution, but it does not seem right that you have to hide coincident constraint markers to get a structure to move and rotate correctly.  If that is an actual official Autodesk way then I couldn't see in the instructions where it says to do that.  

Just checked if I hit F9 to hide all constraints and also turn off "show constraints for selected objects" in constraint settings so the yellow dots don't come back, then I can get things to work more normally, but you still have to grab a vertex and not a line to make a box rotate.