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

[mhag33tg2]

It took a while to find out that screencast used to be the way to make videos, but that's gone and now they recommend Zoom or Slack. Phew, what a trekl!

https://www.autodesk.com/support/technical/article/caas/sfdcarticles/sfdcarticles/How-to-create-vide...

[YannickEnrico]

Ahh, I see what you're experiencing now.

The yellow dots act as constraint markers, and you may notice that you're actually picking and moving the constraint icons rather than the end points. F9 is indeed the way to go.

You may disable visibility of constraints on selected objects here - that way the yellow dots will only show when you press F8

I don't think you can get inventor to rotate a line when you grab a line.

Edit:

I wouldn't expect it to, but maybe that just comes down to personal preference or getting used to the software over the years.

[mhag33tg2]

Yes that is it exactly. I have much more experience with Fusion and with that if you have for example a rectangle constrained just within itself (i.e. no vertical or horizontal constraints) and with only one point on it having a coincident constraint to something else then you can just grab it anywhere, by a line or a corner, and even if the constraints are showing, and you can rotate the whole thing. On that point Fusion is better.

[YannickEnrico]

I guess Fusion is different software for different audience - Also, it's much newer. They probably don't rebuild Inventor from scratch with each new release 🙂

Put it on the suggestions page and they may or may not implement such functionality (I hear it depends on amount of supporters for said idea)

[kacper.suchomski]

1. The program language does not matter. Inventor means icons and hieroglyphs - I learned this program for many years in 6 different languages without knowing any of them. This is not a barrier. You just need to follow and repeat the movements.
2. You can't compare Inventor and Fusion 360.
   These programs have different interfaces, workflows, tools and functionality.
   They have one publisher and several of the same icons.
   Expecting different programs to work the same is a simple way to hinder your learning and development (same SolidWorks, NX, etc.)
3. Coincidence constraints can be made in between:
   1. Any two points (construction point, end of a curve - arc, straight line, spline, etc.)
   2. Point (construction point, end of curve) and curve (arcs, line, spline); this way you will be able to move this point along the curve.
      There is no doubt about it
4. Constraint selection takes precedence over point selection.
5. The F8/F9 keys allow you to quickly turn the visibility of all constraints in a sketch on and off.
   The context menu allows you to turn individual constraints on/off.
6. In practice, the requirement for a correctly defined sketch is 100x more frequent than the rotation of a rectangle, which is why the Inventor interface has programmed response priorities.
7. Dimensions take priority over turnover. Therefore, if you do not create dimensional constraints, the rectangle will be stretched, not rotated. The rotation also requires a constraint defining the rotation attachment; otherwise use the Rotate tool.
8. To analyze cooperation and relationships between geometries in a 2D sketch, it is optimal to use sketch blocks.