Sketch Equal Constraint Issues

[MattPerez314]

When sketching and setting Equal constraints between two lines everything works fine in most cases.  When I dimension one the second instance tends to flip direction or disappear.  This means I have to dimension before placing an equal constraint so it won't flip out.  To compound the issue more the response isn't consistent.  Some cases it will let me change the dimension and work, and others i will use the same dimension on the same sketch entity and it won't.

Example images.  

1. Draw the vertical lines, dimension 5mm and then add an equal constraint. - works fine.

2. Change the dimension to 4mm and the sketch flips out

3. On the "flipped out" sketch change it from 4mm to 6mm and it fixes itself

4. Undo back to the original 5mm and change it to 6mm and it flips out....(won't let me upload 4 but looks just like 2)

[davebYYPCU]

Nothing I can do in a screencast, your sketch when downloaded, 

Fusion has changed your sketch layout to accommodate your request, in your movie, your lines are way bigger than 8mm, so how did you think, 75mm of position lines will fit inside 80mm?

In the movie, you had some short lines, but when setting the constraint, it's important the selection order, Fusion took 25mm to be as the designated value, it made  all 3 the same, you say it's bugged.

To fix it, delete the lower 25mm line.  You need to shorten the top 2 lines click drag  what's left to the right, to less than 8mm and then fusion can do as you want.   Add the bottom line, then make it equal to a top one.  Delete the label dimensions.  Worked for me.

Sketching takes practise to get the correct order of operations, if sketches jump around like yours did, it wasn't constrained well enough not to give Fusion multiple choices.

Luck of the draw sometimes, but Equals Constraint did just that.

Might help.....

[Anonymous]

Hi,

As you can see in the screencast, there was no dimension set for any of the 3 lines. The 25mm that you're referring to is from Fusion, after the equal constraint. So the fact that is doesn't fit in 80mm is Fusions fault, not mine. The file was exported after the fact, no before.

When you use an equal constraint on un-dimensioned lines, selection order should have no impact. And I've also tried different order with the same bug.

The only thing that Fusion should do in this scenario is to make sure that the 3 lines plus my angled "thingy" fit within 80mm and that the 3 lines are the same length. Anything else is a bug.

Regards

Sören

[davebYYPCU]

You got what was asked for, 3 equal length lines.

Didn’t get what you wanted,  - bug.

If Fusion went to 3 shorter lines, forced to fit into 80mm then not a bug?

[MattPerez314]

I played around with your sketch a little bit.  I can't perfectly identify the problem but it does flip the lower line and make it 25.xxxmm long for some reason.  I tried several variations and i think i've isolated it to something with your "show profile" reference and the persistent constraints that are applied.  The way i got around it on yours is to do this.

1. Use Project(P) to bring in the corner points where you want your lines to attach to and then hide the solid body and "Show Profile" in the sketch palette.

2. Draw the lower line from the corner point to your horizontal line endpoint

3. Draw the two upper horizontal lines.

4. Apply your Equal Constraint.

I played with this and the order didn't matter.  You can select all 3 then apply the =, or do the upper two, then the lower or whatever order.  But somehow when sketching those lines when "Show Profile" is on cause the = constraint to flip that lower line.  I tried a few other methods with mixed results.

[davebYYPCU]

If you place all the geometry for the intent, closer to the right side, than left side, does it flip?

Didn’t misbehave in my test / result.

Step 1, was already done, projected profiles without seeing the lines, has been mentioned before.

[MattPerez314]

Yeah Dave.  I tried probably 6 or 7 different workflows to see if i could narrow it down.  I tried to drag the lines to around 8mm as they were in the original sketch, tried to redraw them etc.  it always flipped for me.  It was only when i got rid of the profile/original constraints and solid body that I was able to draw and constrain the lines.

This was one i hadn't seen before.  Usually, like you said, you could drag them close to what you wanted and apply the constraint.   Weird....

[TrippyLighting]

@jeff_strater @rohit.bapat I have not experienced this personally (yet) but there seems some odd behaviors going on in these Sketchs.

[rohit.bapat]

Hello All,

Thank you for the reports and insights. I found a simpler way to reproduce the flipping issue after adding equal constraints.

I have logged a bug FUS-59937 for the team to take a look at. 

However,

while playing with the file and case where essentially we want the tree lines in question to be equal and not go outside the inner rectangle. That to me seems mathematically not feasible. (please correct me if I am wrong)

Here's what I tried to do

Making 3 lines equal using dimensions

In case we want the three lines to be of equal length and remain within the inner box either the Dimension between two slant lines or the angle dimension should be deleted. Here's what I see (I am not using equal constraint here because it is already a bug as I mentioned earlier)
After removing one of the dimension (Angular dimension in this case)

Please let me know if I missed something.

Thank you,

Best Regards

Rohit Bapat

[TheCADWhisperer]

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@rohit.bapat wrote:

...we want the tree lines in question to be equal and not go outside the inner rectangle. That to me seems mathematically not feasible. (please correct me if I am wrong)

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I just set up the same problem in both Inventor and in SolidWorks and the sketch behaved as expected.

[rohit.bapat]

With the dimension between parallel slant lines and with the given angle?

I will have to take a deeper look then. Because I tried to reproduce it using dimensions instead of equal constraints. But, it threw over constrained error which I believe is correct.

Having said that, I will try it in Inventor on Monday. Maybe I am missing something.

Thank you,

Rohit

P.S.

I used the attached model in this thread to reproduce the issue.

[TheCADWhisperer]

I should point out that I used the original *.f3d file that was Attached here. I should have reproduced the entire file from scratch for a valid comparison to the other softwares in my video. I will do that when I get a chance and post the results here.

[rohit.bapat]

Thank you @TheCADWhisperer  for the illustrations. Definitely needs investigation.

I'll play with it tomorrow morning and will ask team to do investigation soon. 

Thank you,

Rohit

[MattPerez314]

@rohit.bapat .  If you take a look at my post and some of the things @TheCADWhisperer did here i had a few steps to follow to get it to behave properly.  There is something off with the constraints in the file and things that are getting automatically applied and not really a user error.  I can't say for sure what it is behind the scenes but the application of parallel constraints on the short lines and some underlying references i feel are the key.  In the situation where the 3 lines in question are equal, the distance of the two upper lines plus the width of the parallelogram is equal to 25.236mm.  The "flip" line situation is 25.729mm.  I can't figure out why/how Fusion tries to make each line 25.729mm long.  Nothing else in the file comes out to that number.  The horizontal distance of the parallelogram is 8.083mm.  The box inside edge is 80mm.  Its thickness is 20mm.  

I made a screen cast based on the workflow i tried to make it work.  Hopefully it helps you replicate the behavior.

 

[TheCADWhisperer]

@rohit.bapat 

I should have attempted to recreate the Fusion 360 file from scratch before making video.

I just go around to doing from scratch rather than using the original file attached previously, and Fusion 360 behavior worked as expected - same as Inventor and SolidWorks.

So there must have been something in the way the original geometry was created that was causing this unexpected behavior.

[Anonymous]

Maybe I should give a little background to how the problem started...

I was making a triangulated steel truss design. Something like this

To build each section (a / followed by a \), I made the "/" part and mirrored it to get the "\". Since the spacing between the "/" and the "\" was to be the same as between each section I needed the double line with the equal constraint. That's when the problem occurred.

To figure out what the problem was, I boiled it down to the "Equal constraint demo" file and uploaded it.

So, here I've attached the same file but before the application of any constraint. Hope that helps.

Regards

Sören

[jhackney1972]

It is such a joy to read comments from satisfied users of Fusion 360.  We hope you will continue enjoying the software and come back to the Forum often to post your delightful comments.

[TheCADWhisperer]

 the fact that seasoned users stay away of features because they never know when it will ruin everything--

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@mbstoops 

You have not presented any facts.

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

And describe any issue that you encounter.  Any factual issue.