How do you delete Coincident Constraints?

[scottmoyse]

So how do you delete the coincident constraint between two rectangles? or even between two line segments of a rectangle?

[Oceanconcepts]

In your example I can delete the upper coincident constraint by highlighting it and pressing DELETE- then I can move the vertical line independently. 

I can delete the parallel constraints on the rectangles, and move the corners. 

I can draw a rectangle constrained to another with a coincident constraint, delete that, and (by highlighting the desired sketch curve with a long press, then using the Move tool), separate the two rectangles. But I don’t see any way to separate the corners of the rectangles, short of deleting a line and re-creating it.

[scottmoyse]

I highlighted the coincident constraint to show that it is there in that condition (and can therefore be deleted), but it isn't present in other conditions.

The coincident constraint between my two rectangles was inferred on creation. Are you saying that if you manually create that constraint between the two rectangles, then you can delete it? If so, the fact that you have to create the constraint manually just to delete it sucks, which I'm certain you would agree with.

Deleting objects in sketches is to be avoided where ever possible when using history based parametric workflows. It just breaks downstream features which needn't be broken.

Cheers for helping to clarify my point.

[Oceanconcepts]

I was able to get the coincident constraint to just appear by drawing a line in that position, I didn’t manually create it. I could delete that one, but the rectangles appear to have an invisible coincident constraint that can’t be deleted. Even deleting the parallel constraints leaves the corners of the rectangles pinned together, with no apparent way to unstick them. So yes, that seems less than optimal behavior.

[scottmoyse]

any chance of doing a screencast to show what you mean with drawing a line to expose the coincident constraint between the two rectangles please?

[Oceanconcepts]

Scott, I’m afraid I may not be clear. I was able to get the constraint symbol to display when I just drew a line, but it was a constraint for the line. Ditto when I draw a rectangle that doesn’t involve a corner. But when I use a corner point for a reference, I don’t seem able to alter the relationship, and it’s not displayed as a constraint. Maybe this sin’t what you were referring to?

https://screencast.autodesk.com/Embed/Timeline/ea61f9f2-7d28-424a-aa23-6f8cd399ab1e

[Anonymous · Accepted solution]

Hi Scott,

You should be able to delete nonvisible coincident constraints by clicking/selecting on the relevent point, then right clicking the mouse and choosing the option that should show up called Delete Coincident. 

Sometimes there are multiple points superimposed upon each other, so to select the correct point(s) to delete their coincident constraint(s) you can hold the left mouse button down on the point until a list of superimposed features comes up, and try each point available.  You should not need to do that for this case though.

Jesse

[Oceanconcepts]

Thanks, Jesse, that will be very useful. I had not come across that before. 

[scottmoyse]

I've just created this video showing your solution:

Thanks!

[scottmoyse]

To be honest... I feel a bit stupid, because although you can get the coincident constraint glyphs to show up in Inventor, you can delete them in the same way from the context menu. Sometimes its the only way to delete them. 

In Inventor you can right click on the end of a line element of a rectangle and it will delete the coincident constraint at that end. You can't do that in Fusion, but it would come in handy at times in complex sketches. That way you don't have to fumble around in the Select Other list.

[Anonymous]

Thanks for that video, and it made me realize you can add coincident constraints back by just snapping the ends together, as apposed to using the sketch pallete. 

That's also a real good idea using the lines to remove, or even apply coincident constraints to endpoints, as that can get pretty hairy at times. 

Jesse

[jeff_strater]

Great topic, everyone.  Thanks for bringing it up, Scott, and Ron and Jesse for providing the answer.  Now, I can add the justification, and more about the internals of Fusion than you probably ever wanted to know.

So, the obvious question here is:  Why don't we show a coincident constraint at the corners of a rectangle?  Mostly it's for clutter control.  Can you imagine what a sketch would look like if every junction had a visible coincident constraint?  So we made a rule:  Don't show coincident constraints when there are two or more lines sharing the same endpoints.  Also, because we are fussy technical types, we did this because it reflects the internal data model as well.  When you create a rectangle, there are just 4 lines and 4 points involved.  That is, the 4 lines "share" an endpoint at each end.  There really is no coincident constraint there.  We could have implemented it as 4 lines and 8 points, with coincident constraints between pairs of endpoints, but then the data model gets messy, and there are more points and more constraints to deal with internally as well as externally.  For what it's worth, this is the same implementation as in Inventor (most of us worked on Inventor too).

But, then, sometimes (like in this case), you do want to pull apart the rectangle.  So, that's why we put in the "Delete Coincident" command into the context menu.  (and, just FYI, Scott, you can get this command on a selected line as well as a selected point, like Inventor, and it is sensitive to what end of the line you selected).  This command makes it look like you are deleting an invisible constraint, but what is really happening is that we are adding a new point to the sketch, and pointing one of the lines to it.  If you select the point to do this, we just pick one of the lines (if there are more than two sharing the same point), if you select a line, then it's obvious.  The points are then on top of each other, and if you drag one off, the lines will separate.

If you drag one point on top of another, the inverse happens:  We merge the points.  So, if you are not careful how you drag you can:  1)  Delete Coincident 2) drag the points apart 3) drag them back together, leaving you exactly where you started.  

Fusion does not merge the points if they just happen to sit on top of each other for other reasons.  For instance:

The result is two points sitting on top of each other.  Yeah, probably too much information...

The last interesting thing that is somewhat related:  In Fusion, you do not have to have the coincident constraint for Fusion to recognize a profile:

Hope this was enlightening in some small way

Jeff Strater (Fusion development)

[Oceanconcepts]

Thanks, Jeff. That does help me understand some occasional frustrations in sketching. For me it’s often when sketching a spline- if the point I create just happens to land on another, then I’ve been stuck if I wanted to change it. Now I see I can remove that constraint and edit the spline further. That is really very helpful.

[scottmoyse]

Very interesting. Thank you for making sure it behaves the way you show in the last image. I have noticed that. Please can you show me where I can delete the coincident constraint from the line? I can't get to it:

[scottmoyse]

Regarding not cluttering up the view with constraint glyphs, the way that is dealt with in Inventor (Since 2015) is they only appear when you select the point. It would be more discoverable in Fusion 360 if that were also the case. 

For reference, here is a screenshot showing the Delete Coincident Constraint option in the line element context menu:

[jeff_strater]

Hmm.. it should be there when a line is selected.  One thing that we are in the middle of changing for Fusion:  Right click does not select.  So, try selecting the line with left click, then do right click.

Here's a short screencast showing how I did it:  http://autode.sk/1LabBTr

Hope this helps

Jeff

[scottmoyse]

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@jeff_strater wrote:

Hmm.. it should be there when a line is selected.  One thing that we are in the middle of changing for Fusion:  Right click does not select.  So, try selecting the line with left click, then do right click.

Here's a short screencast showing how I did it:  http://autode.sk/1LabBTr

Hope this helps

Jeff

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YES!! which is actually consistent with the point as well. Silly me. But I would imagine it would be an improve to select on right click as well... 

What are your thoughts about the Inventor Coincident point display method?

[Anonymous]

That is so awesome the Delete Coincident is also available on lines, arcs and splines, and is sensitive to what end of the curve the action is performed!

I'm pretty certain when you say you can delete a coincident by dragging (your #1 listing) you mean that Delete Coincident must first be performed.

Thanks Jeff for the great info!

Jesse 

[jeff_strater]

@Anonymous:  Yes, I did mean that you need to Delete Coincident first, before you can drag the lines apart.  Good catch.  You cannot break lines apart by just dragging

@scottmoyse:  Yes, the Inventor way of showing these constraints actually works pretty well.  That's a pretty good way to show these without normall cluttering the display.  We are also considering a way to let the user show or hide constraints on the whole sketch, because sometimes they are useful, but sometimes they just get in the way.  When constraint display is off on the whole sketch, it would make sense, then, to show the constraints of the selected geometry.  

Thanks again for the great input.

Jeff

[scottmoyse]

@jeff_strater To be honest, the way Inventor handles constraints across the board in the sketch environment is excellent now. It wasn't pre-2015 but they've really nailed it now. F8 & F9 toggles constraint displays (based on constraint display settings) and as soon as you select any sketch object it's constraints appear. If you window select objects, again all their constraints appear. The relax mode is epic as well! 

When it comes to reviewing this lot, have a good look at Inventor 2016 sketch constraints. I'm sure you would anyway.