Dimension tool is slowing sketch editing to an unusable speed

[Anonymous]

I have a relatively basic project - basically a flat surface extruded to 0.25" and cut into a few different shapes to make a box out of. Two of those shapes have some holes extruded through them, and text extruded into them, but not through. So there are a lot of dimensions going on, but still fairly basic. I still need to make several more holes with dimensions and, while sketching the holes is fine, when I use the sketch dimension tool, I get the spinning beach ball (on Mac OS) and it is very hard to get anything done. This project has been fine for me for a few weeks, but has recently started doing this. I have made several projects before this that are similar. I have not (to my knowledge) updated anything.

Is this because text is too demanding?

If anything is needed to understand my situation, please ask me.

Thank you!

[jeff_strater]

we'd have to see the sketch in question, but yes, the larger the sketch gets, the slower the solve is.  Two ways to improve the solve performance are:

1. turn off profiles.  Computing those profiles is expensive.  Turn it back on when you are done editing:
   
2. if there are areas of your sketch (e.g. the text) that you won't be editing, dimensioning, select those, and Fix them.  This will keep them out of the solve process totally.

[Anonymous]

Thanks for your reply! 

By fixing a sketch, do you mean using the 'fix' constraint (i.e. the red lock)? I can do that, as well as hide the profiles of any other sketches, but I created a new sketch where these new holes will go, so not sure if fixing a different sketch or hiding the profiles of a different sketch will improve performance? Also, when this happens for me, the application itself is 'not responding'. 

[TheCADWhisperer]

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

[Anonymous]

Sure! Since you responded I 'fixed' the three sketches 'surfaces', 'controls' and 'rear jacks', and 'sketch 7' is the one I am currently working on that is giving me issues

[jeff_strater]

yes, by "fix", I meant using the Fix/Unfix command:

An important thing to understand about "not responding".  Operating systems will periodically ping applications.  If they don't get a response, then the "not responding" dialog is shown.  However, it could be that the application is just really, really busy, and has not had time to respond to the ping.  So, if you have a very complex sketch, Fusion is likely just using all of its resources trying to solve that sketch, or find the profiles.  In many (most?) of those cases, if you just wait it out, Fusion will eventually finish.

[jeff_strater]

thanks for sharing the file.  I looked, part of the problem is that sketch has 1200 curves and 1200 points in it.  That's because you've created the sketch on this complex face:

with :auto-project geometry on active sketch plane" on:

Every tiny edge will add a sketch curve to the sketch.  I believed that this is what is slowing down this sketch.  Selecting and deleting that geometry helps a bit.  But, still the performance is not great, even when the sketch has under 30 circles in it.  I need to send this over to the sketch solver team to try to figure out why it is so slow.

[edit] the Fusion bug to track this is:  FUS-73024

[Anonymous]

Thank you so much! Is there a better way to create words in something like this? This will be realized by a CNC machine, and it will be made out of baltic birch plywood. I want to avoid using something like stickers for the words, but the labels are still needed since there are so many different controls. This was the way I came up with but I am open to alternative methods as well

[jeff_strater]

no, I don't think there is anything wrong with what you are trying to do here.  Cutting those words into the body should be fine.  I think the problem here is really on the Fusion side - even with those curves removed, it takes a very long time to add dimensions to a relatively small number of circles.  That should not be the case.

I'm not really sure how to tell you how to proceed.  I assume that all you really want to do here is to position those circles using dimensions.  You might be able to get better performance if you just use Move to position them, but that seems like a wrong approach, since you want to be able to edit the dimensions.  You can, though, still use Fix to lock down circles that are already positioned.  The dimensions will still exist and be editable when you Unfix those curves.

Let's see if the dev team can come up with other recommendations...

[jeff_strater]

just to let you know we have not forgotten you, @tan.c.stowell .  This is turning out to be a bit of a mystery.  It is not clear what pathology is causing this slowness in Dimension, but it is definitely there.  It does seem to be related to all the projected edges in that sketch, but not to the ones at the top of the sketch, because if I delete those, the problem still occurs.  We are investigating.

I did find a workaround:  deleting ALL the projected geometry, then selectively re-projecting just the 3 edges you need to position the circles on that face.  After that, Dimension seems to work fine.  I have no idea why.

Thank you for sharing the design with us, and helping to identify this performance problem.

[Anonymous]

Awesome, thank you so much. I really appreciate all this help. I was able to get it to be usable enough for me to get the dimensions I needed to get, by implementing the various tips you had previously mentioned. I also found out during this experimentation that if I highlighted the two edges I wanted to dimension first, and then select the dimension tool, it worked with much less delay.

I was also wondering if it is more or less or similarly demanding to dimension everything or to use constraints like equality and co-linearity in place of dimensions where I can

[jeff_strater]

@Anonymous - using pre-select is a good trick.  I hadn't thought of that.  But, it does help verify what seems to be the issue here.  The slowness is not in the solve of the sketch, but has something to do with the dimension command itself, looking for valid things to select.  If you pre-select the circles, then the command skips this step.  So, good find there.

regarding:  "I was also wondering if it is more or less or similarly demanding to dimension everything or to use constraints like equality and co-linearity in place of dimensions where I can".  This is something I've wondered about myself.  I have never done an exhaustive study to find out the answer, but, every experiment I've done seems to show that it doesn't matter.  Dimensions, equal constraints, Colinear constraints (your use of Colinear here is very interesting.  To be honest, I didn't even know you could use Colinear that way...) horizontal/vertical, all seem to be about the same as far as performance goes.

I would probably use Horizontal/Vertical in this case (select the circle centers you want to be aligned, and make them horizontal to each other), or just draw a horizontal construction line, and use Coincident to constrain the circle centers to be on that line.  But, I think any of these approaches are valid.

Glad to hear you were able to make progress on your design.