Alan B
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| posted on 30/11/06 at 04:45 PM |
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Solidworks weldment question
I've been practicing with weldments to good effect and been able to save the seperate bodies as individual parts (they are round tube and
compound angle fishmouths).
My question is how can re-orient the palnes on the parts so as they make sensible views when I create drawings? As of now they are just picking up the
planes from the original weldment model.
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balidey
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| posted on 30/11/06 at 04:57 PM |
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Not the 'most correct' way, but get the model open, click on the face you want as the default, click to view as 'normal to'
and then create a drawing sheet. When entering the model view, use 'current model view' (Not top, or front etc) so you now have a view
looking straight on your datum face, then you can pull other views off at 90 degrees. Make sense?
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flak monkey
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| posted on 30/11/06 at 05:00 PM |
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Its a pain in the arse, you can re-orientate the part by drawing axis through it and using plans to turn the part into a sensible direction. Its a pig
of a job and something I have suggested that solidworks try to sort out for their next release. Doubt it will happen though, but the moan made me feel
better 
Sera
http://www.motosera.com
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Alan B
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| posted on 30/11/06 at 05:01 PM |
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Yep, makes perfect sense. You'll just have to careful not to move the model I guess.
I don't have a single flat face on some parts so I guess I'd have to try and get round that....I can put some axes in so maybe that may
help.
Cheers
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balidey
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| posted on 30/11/06 at 05:19 PM |
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Or if you are worried about rotating the model in between operations, set the view you want and then save that view in the little
'orientation' box, then 'i think' you can load these custom views into drawings
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Alan B
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| posted on 30/11/06 at 05:29 PM |
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Ah Ok.....yeah...another good tip.
Thanks everyone.
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bigandy
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| posted on 30/11/06 at 07:35 PM |
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I've had a moan about this to SW too. It's a right pain trying to reorientate a part to the default Origin/reference planes.
What I tend to do is either create a new set of reference planes to use to creat drawing views from, by inserting them int he correct place in the
model.
The other way is to set the model viewport up so you are looking at the model as you want a drawing view, then save that view (space bar to bring up
the saved views menu). WHne you create the drawing now, one of the options when creating a new model view, should be the view that you saved
previously.
Or, if you are in a hurry, you can just orientate the model how you want the view to look in the drawing, then when inserting a new view, just select
"use current model view" to create a drawing view that replicates the current model view. You can run into problems doing this though,
especially if you come to update the drawing at a later date when the model has changed.
Cheers
Andy
Dammit! Too many decisions....
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DorsetStrider
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| posted on 30/11/06 at 08:03 PM |
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At the risk of of hijacking the thread...
Would anyone be prepared to ...erm...back me up a sopy of solidworks that has the weldaments feature in exchange for a ford technical information
cdrom?
PM me
Who the f**K tightened this up!
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jono_misfit
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| posted on 30/11/06 at 10:06 PM |
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I think the technical drawing bit of solid works really lets it down. Ive got 2005 and its pants.
At my placent they use NX2 & now NX4 (Which i found a pain to model with to start with) which is great for doing drawings with.
I think it almost ruins it considering how easy the rest of the package is
(cough) use Emule (cough)
[Edited on 30/11/06 by jono_misfit]
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flak monkey
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| posted on 30/11/06 at 10:11 PM |
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Nice avatar  
Sera
http://www.motosera.com
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liam.mccaffrey
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| posted on 30/11/06 at 10:15 PM |
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isn't it!!
Build Blog
Build Photo Album
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bigandy
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| posted on 30/11/06 at 10:24 PM |
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SW2006 is a little bit better, and I've heard rumblings that 2007 has improved things slightly again, although our IT department won't let
me loose on it just yet 
Cheers
Andy
Dammit! Too many decisions....
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jono_misfit
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| posted on 30/11/06 at 10:39 PM |
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I quite like it, need to re-size it a bit though....
I got 2006 about a month back, but too busy to clear space and install it. I had to send a drawing of to get tubes bent the other week. Took me ages
to get a dimension to the centre of the bend arc (if that makes sense). Its about 2 clicks on NX4, and Catia's just as easy as well.
Think this is how they save on the packages.
Back to the original question. Can you save a blank sheet with a fixed view and import the parts in (saving a copy each time) to get the required view
in the drawing package?
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bigandy
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| posted on 1/12/06 at 10:04 AM |
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Re: dimensioning the bend. Depending on the complexity of the bend, and the orientation of the drawing view are trying to dimension it in, I would
probably do it one of two ways.
One way is to create a centreline beween the two edges of the tube, and dimension this (will only work if the view is normal to the bend plane).
The better way would be to create an axis along the bend path in the Model, either a reference axis, or sketch. You can then dimension this in the
drawing. I'm not sure how you have modeled the bent elements in the first place, but it could be that you already have this line drawn in the
model, and have used it to create the structural member, in which case just use that line (you have to make sure the weldment profile is centered on
the line though, otherwise you would not be dimensioning the centre axis of the bend )
I hope that makes sense!
Now, regarding the drawing views, then you can set up default views to be created in a new drawing, the easiest way is to set up a drawing template,
with the views you require already present. I have never really seen the need to do that in my work, as I find it easier to have a generic template,
and insert the appropriate model views when creating the new drawing manually.
However, what you need to do, is create a new blank drawing (using the sheet format of your choice) and instead of inserting a model view, insert a
predefined view. You can then set this predefined view to be of a number of standard views (eg top bottom etc) or a custom one if you have set it up.
You can also then create projected views of the predefined view if required.
You then need to save this drawing as a Drawing template (file, save as, draiwng template), in the folder you use for drawing templates.
Now, when you have the part open that you wish to populate the drawing with, just click on the "make drawing from part/assy) button, and make
sure you select the drawing teplate you just saved. This should then populate the drawing with the views you set up.
It can take a bit of time and tweaking to get it displaying the exact views that you want, and a bit more time setting up the custom views if you are
not using a standard view (top bottom, etc) as the "predefined view".
I tend not to use this method much, if at all, as it doesn't really save that much time when creating drawings (at least in the work I do most
often). It probably is of use if you ahve a large number of similar drawings to do though.
Hope that helps a bit..
Cheers
Andy
Dammit! Too many decisions....
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