angled dimension in projected view

[dgowans]

I'm having a brain cramp and can't find this in the help anywhere.

I've got a projected view of a part that I'm dimensioning. I want to add a dimension like the one circled in the attached JPEG, but I can't do it without first adding circle centers that are at an angle to compensate for the angle of the view projection.

Is there any way to simply add the circled dimension by selecting the arcs at the end of the slots? Every time I do this I can't get the angle of the dimension to come out such that I get the value I care about, no matter where I place the dimension. The dimension either snaps to the shortest value between the slot ends or horizontal/vertical with respect to the part model. What I want is the dimension as it's shown and it seems I should be able to get it without resorting to dimensioning the circle centers.

Am I nuts?

 

[TheTick]

Add a centerline between the slot sides of the lower slot. The line will control the dimension's orientation.

I think it may be possible also by selecting the ends of the centermarks.

 

[dgowans]

Tick,

I can get the dimension in the orientation I want if I add properly oriented centermarks and dimension between them. What I'm asking is if I can do it without adding the centermarks.

It seems strange to me that I can add centermarks at a specific angular orientation but I can't do the same with a dimension.

 

[handleman]

The centerpoints of two arcs are just that - points. How should the software know what angle the dimension is put in at?

 

[dgowans]

It shouldn't know, but it should be polite enough to ask...

Like I said, I can't figure out why there's an option to place a centermark at a specific angular orientation when you can't do it with a dimension. Unless, of course, the point of being able to orient a centermark is the method by which I can achieve my oriented dimension.

This works in my case but does nothing for the case where someone would want to dimension between two random points (not circle centers) at an angle that's not square with the part's world.

 

[mncad]

You should be able to pick the 2 points and then move the mouse around and it will give you the 3 different dimensions, horizontal, vertical and a rotated, at least in SW2007 anyway. I know this will get people fired up but..... in ACAD its called a Rotated dimension. You can pick any 2 points you want with the dimension command, then pick Rotated and any 2 points that you want (either the same or different from the first 2) and those will set the rotation of the dimension.

mncad

 

[dgowans]

Yep, the rotated dimension is what I'm looking for...

 

[fcsuper]

Rotated Dim in ACAD, at least when I used to use it, didn't work well. It almost always assumed the wrong rotatation angle.

However it would be nice to have something like that in SolidWorks, where a user can choose the angle by selecting a parallel line or something.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[Timelord]

dgowens,

I have had this issue also. The solution I would use is to draw a line between the arcs that form the aligned slot ends and then dimension that line to the upper arc and then hide the line.
When you dimension to points (arc centers), Solidworks always give you the shortest distance or the horizontal or vertical. Dimensioning to a line, Solidworks assumes it represents an edge in a drawing and then only gives you a dimension perpendicular to that "edge" to another entity. When you added centermarks that were rotated to the correct angle, you gave SW an "edge" to dimension to (actually two "edges" and I bet on occasion you select the wrong line from the center mark and have to reselect). If you know this behavior, you can exploit it as in my solution. It appears that SW does not redefine horizontal and vertical in a rotated view such as you have shown. If it did, the centermarks would come in aligned as you have shown at an angle of zero and dimension would be aligned like you want when you just select the arcs. My solution is optimal because I drew a line that is tied to the direction I want the dimesion to go and will update correctly if the rotation angle of the view is changed in its parent view. The centermarks will not update because they do not auto rotate with the view.

Timelord

P.S. I am still on SW 2005 SP5.0 and I assume from your problem that this has not been fixed, at least up to the version you are using.