dim question

[ParaCAD]

Can you insert dimensions from the model in to a draft instead of creating dimension directly in draft? Thanks in adv.

Adam
Solidworks 2005 SP01.1
Windows 2000

 

[beachcomber]

Yes.
It's the 'Retrieve Dimensions'command - the icon is a dimension with a hand on it.
There are options in the command as to what types of annotation get inserted.
I've never really used it because the dimensions required for drawings are not usually the ones you've used to model it.

bc

 

[ParaCAD]

AH...thanks.

Adam
Solidworks 2005 SP01.1
Windows 2000

 

[KENAT]

Paracad

Unfortunately retrieve dimensions doesn't work that well, you'll find it doesn't retrieve all dimensions and won't always let you put them on the view you want.

This was brought up at the round table at PLM world as a requested improvement.

That said you can develop a methodology to maximize it's usefulness, if you want more details ask in a post and I'll come up with what I've been doing recently.

beachcomber

I'm slightly surprised by what you say in your message "the dimensions required for drawings are not usually the ones you've used to model it". Surely having the drawing dimension scheme matching the model scheme better captures design intent. It also makes changes from redlined drawings easier and of course facilitates use of retrieve dimension. I know it's not always 100% possible but I always try.

In fact we're looking at introducing it as policy in our Design Room manual.

I'd be interested in other users views.

Ken

 

[fwc]

You may not get what you want, if you create the dimensions on Right View (in part) but retrieve dimensions from Left View (in draft).

 

[beachcomber]

Ken,
I agree it would be nice, but I think it would be damn near impossible to model a part (other than a really simple one) where ALL the constraint dimensions are the manufacturing dimensions.
Instead of 'not usually' I should have said 'not always'.

The other thing with retrieve dimensions is that if you put a tolerance on the dimension in the model any changes to that tolerance will not be reflected on the drawing.

bc

 

[ParaCAD]

KENAT - I like to read what your doing

I've always tried to model using dimensions that I know I'll want to use in the drawing. As stated it isn't always possible. But it is nice to try. The fisrt 3D cad I used in my everyday design was Pro/e, then moved to SW and now SE. Out of the 3, Pro/E seem the most complete when it comes to using model items in drawings. It seems that feature is just less important to develop or improve in SW & SE. my thoughts.

Also thanks all for the advice. I'm in a crunch to learn all I can about SE.

Adam
Solid Edge V17
Windows XP Pro

 

[KENAT]

ParaCAD

I don't have time right now, I've spent far too much time on these message boards the last couple of days, but I'll try and put something together over the next couple of days.

I learnt SE & Pro E at about the same time, I never had formal training on SE (unless you count a couple of short sessions at a conference) but did for Pro. I've got to say I much prefer SE, even being self taught I'm a lot better on SE than Pro and find it much easier to use. That said Pro does support, encourage and to some extent force the model to match the drawing, which I've come to realize is probably a good thing.

Trying to use the dimensions in the model that you'll use in the drawing can take a bit more thought and effort for all but the simplest parts but I like to think it's worth the effort and better reflects the design intent. This is especially true when you're trying to apply GDT and making the drawing support inspection. Just my thoughts and from what little I've seen I don't think SE training fully supports this which is a shame. They seem to focus on what the software can do, not what you should do with it, if that makes sense.

 

[KENAT]

ParaCAD.

My entry on this subject in our draft Design Room Manual just got blasted so I'm going to have to go over it and make it a bit more bullet proof for our use anyway. When it's done I'll try and post a version of it.

Ken

 

[ParaCAD]

Sounds good I appreciate it.

Adam
Solid Edge V17
Windows XP Pro

 

[KENAT]

I haven't forgotten, just crazy busy, they can't decide what standards to work on first amid the general panic!

Basically,

Use dimensions in the model that you want in the drawing, I tend to treat the model reference plance like datums ABC on the drawing and dimension accordingly.

Place the views on the drawing you think you need.

Select what you think will be your primary view and retrieve dimensions on it. Rearange and delete any you don't want in that view. (Do not manually add dimensions at this stage).

Repeat this on the next view, and the next etc.

Once you've retrieved dims for all views, deleted and tidied up accordingly then manually add any missing dims.

Hope it helps, I used it quite a bit on my last project. Some parts it worked well others it was a bit of a hassle.

Ken