Hi! I've got a problem with a dimension tool. I need to set a distance between to rectangles with rounded corners. I used to do it like on the attached gif. But not, everytime I try to do so, I get degrees instead of distance and I have no idea of how to change this. I thought it might be because of some constraines so I removed all of them but it didn't help. What might be the reason for this?
A problem with dimension tool. Degrees instead of distance
If you come across something like this export the file as an f3d and attach here. If you can't share the whole design delete everything apart from the problem sketch.
Thanks Mark
Mark Hughes
Owner, Hughes Tooling
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Hi Konstantin -
This is happening because those two lines are not parallel....(even just that tiny bit). We have a dimensioning tool that tries to recognize what you want to do in different situations, and since two non-parallel lines don't have a constant distance between them, you'll get an angle from the tool.
Add a parallel constraint to the two lines and it should fix it up.
Now - the next question is, why did this happen? Especially such a tiny amount. This is going to be tough to answer without looking at all the steps you took to get there - but my guess is that you deleted the parallel constraint you had on these lines before, and probably unintentionally dragged some other piece of geometry which was related to one of these lines by some other constraints! Whew!
Since its not clear how you got here - you may have unintended results when you add the parallel constraint back to these lines. (I hope not - but it can happen) You'll have to work backwards if that happens to fix it.
How to avoid in the future: BIG TIP - it is a good idea to make your sketches SIMPLE. Better to have multiple simple sketches than one magnus opus. (uh - that's a really complicated sketch.) This will help you avoid unwanted relationships and missteps and it has the added benefit of really improving the performance of your software. (Sketches are one of the biggest performance-draws on your system!)
Second tip: Sometimes, it can be best to turn OFF automatic inference of constraints. You can do this generally in your sketch options or temporarily with the control key (I think thats what its called in English. I use the German). When you do this, an old trick is to purposely draw your sketch all out of whack - and then use the constraints to PURPOSEFULLY bring it into shape. Then dimension it.
Using these kinds of tricks will help you avoid this sort of headache in the future. Mostly. Sometimes....stuff happens. Good luck.
Mickey Wakefield
Fusion 360 Community Manager