Dimensioning at non-orthographic angle

I need to dimension objects that are at an angle.[see attached
image] In AutoCAD I would rotate my UCS so that it was parallel to the
object I was dimensioning and then the dimensions would be aligned with
the edge. I can't simply dimension one edge because it would not give
me the overall length. I wish I could attach an image (Google groups
doesn't allow it)

At the moment, I cannot find any method in SW to do this with just
dimensions. I can create a sketch on the sheet, and create a
construction line and constrain it to be perpendicular to one of the
eges. This sketch line would become my extension line, but that would
be a lot of work for something I must do a lot of.

Any ideas?

Joe Dunfee

 

I may not understand something in your message, but if you plop in an
isometric view, it asks you if you want to have projected or true
dimensions. If you choose true, you can just put in real dimensions.
Sometimes the witness lines won't go the way you want, but at least they are
correct numbers. Is this what you are looking for?

WT

 

The object I am dimensioning is a weldment of square tubing. The
tubing is at odd angles, some acute and other obtuse. If the tubing is
laying horizontal or vertical, I can dimension it easily by selecting
the most extreme points. Below is an example in ACSII art; (View with
a monospace font like courier)
_______________________________________
/ , '|
/ , ' |
/ , ' |
/__________________________, ' |
| |
| |
|<-------------------1' 2"--------------->|

If the part is oriented horizontally as above, I can dimension it. But
if the part is tilted a bit, then if I dimention to the extreme
corners, I only get a diagional measurement, not a dimension aligned
with one of the long sides.

Joe Dunfee

 

Sounds to me like you're doing about the only thing that would work
(with sketch lines). Cumbersome.

 

You could - in the part environment - position your model so it is
shown the way you want (use "normal to" and shift / Ctrl / Alt with
arrow keys). Then press Space and define a named view. Make a new
model view in your drawing, and if it is alligned correctly it will
display the correct dimension.
Feel free to mail me your part and drawing if needed.

Thomas Voetmann

 

In the case where the part is simply not alligned to one of the
standard planes this can be done in the part.

In the case where you are trying to dimension features which do not
show their true length in any of the standard orthographic projections
it is necessary to create an auxilliary view in which the feature is
shown in its true length.

It might also be possible, though not standard to show in an
axonometric projection and choose true length instead of projected
length.

 

Thanks for the suggestion, but in this case the part is a weldment.
I can't create a view of a single member of the weldment. I will
e-mail you the test drawing I created, but I suspect that I am stuck
just drawing construction lines which are what I dimension to. I just
finished a more elaborate part done this way, and it wasn't so bad
because the angled parts are only a few pieces out of the whole.

Joe Dunfee

 

Joe,

You can create a view of a single weldment part.

Search in the SolidWorks help for "weldments, weldment drawings"

Hope this helps.
CG

 

is this what you want

|<--.500-->|
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There are 3 dimension tools There are Horizontal, Vertical and Smart to
get a dimensionlike this you could do Smart or Horizontal. Select the
line and drag the dimension up beyond the top point of the line and
then move it to the right until the dimension priveiw snaps the
direction you want or drag down to the left to get the Vertical. If
you RMB and select more dimensions you will see the horizontal and
vertical dimension tools these work on angled lines with no fus.

If this isn't the case you should project auxilary views to get a true
view of the desired objects (this would be the correct method from a
drafting perspective). Or you can cheat and create a true view in the
model and save it as a named view. Then you can create a new view
using that named view.

Corey