I am trying to add an arc length measurement to a curved part on a drawing. The method suggested by SW Help works on sketches, but not on a drawing. Any suggestions/
So I have done some testing and found that up until SolidWorks 2014 to dimension the arc length in both a sketch and drawing you could select the points first then the arc, select the arc first then the points, select the arc first then control select the points.
Starting with SW2015, dimensioning the arc length in a sketch had not changed but in a drawing the points much be selected first (control key optional) then the arc. I looked through the SW2015 help but could only find what Steve and Lesley found about sketches.
Unless the settings are messed up on my computers...
If I get a chance tomorrow, I will scan through the SolidWorks Knowledge Base to see if this is documented.
You can use the sketch dimensions in the drawing.
2017 SOLIDWORKS Help - Model Items
Try selecting the end points of the arc first then the arc.
If you've already dimensioned the arc in the sketch why not just use that dimension in your drawing?
if you need to, just select the arc and then ctrl + select each endpoint of the arc, that should give you what you're after.
What version of SolidWorks does that work in. My screenshot above is from a SW2016 drawing. If I try your method I get "Could not create..."
Perhaps I'm mistaking, I'm at home and don't remember the exact selection but I'm not far off I'd bet.
I'm using 2015 at work and that was from memory but here is the 2016 help files.
2016 SOLIDWORKS Help - Creating Arc Dimensions
Interesting read. In the 17 years I have been using SolidWorks, I have never pressed the ctrl key. I will have to research it more to see what SW is trying to get at.
None the less, it does not work on non-sketch arc in a drawing. As I stated in my original post you must select the arc first and then the end points (without the ctrl key pressed); at least that is the way it works on my computer????
You have me curious now. I will have to fire up SW2012, 2014, 2015, 2017 and beta3 and see if it works the same. If I have time I will fire up SW2001+ to see if it was different way back then.
I want to thank all of you for your responses. I tried Steve's solution and it worked. You have to select the two end points and the arc with the CTRL pressed to generate the arc dimension in a drawing. This works in SW2017. I have not tried it in older versions.
I tried the above method without using the CTRL key and it works to generate an arc dimension in a drawing.
Thanks again for all of your help.
selection order shouldn't matter. I can select points first then arc or arc first then points and it works both ways, no CTRL key needed. SWX 2017
Roger, we are talking about an arc length in a drawing not in a sketch.
Top dimension is 2 endpoints then arc, bottom dimension is arc then two endpoints.
Interesting. I just happen to have a part similar to yours. And I can select the arc first then the points to create the arc length. I could also do it on the fillet. However, it did not work on the keyway (will if I select the points first). Have you tried using this method on other parts to see if it always works for you?
The arc on the key way is a 3D line, so the arc isn't really an arc, it will be a spline curve?
you should be able to dimension the bottom curve of the slot though??
Sorry for the misunderstanding. It is not that I cannot dimension the arc length of the keyway end (see below), the issue is the method used to create the dimension (see previous posts by myself and others). SolidWorks seems to now have two sets of rules for dimensioning arc lengths whereas prior to SW2015, it only had one.
generally when viewed normal to, an arc is an arc even if it is on a curved surface
or try creating a sketch in the drawing sheet using that 3D arc??
that should dim up nicely??
Figured it out. You can select the arc or the points first when dimensioning the arc length of a silhouette edge but you must select the points first when it is not a silhouette edge. Very confusing...
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