Redefine Coordinate System? 2

[Browndoff]

How can I PERMANENTLY redefine the coordinate system in Solidworks? I want the Z-axis to point 'upwards' [as usual outside Solidworks] for ALL my future models - to eliminate hassle having to re-orientate models before 'exporting' the files to suit clients' CAD format! I'd like to be able to view my assemblies in 'true' Isometric form on any CAD system!
If that's NOT possible - is there a 'macro' which will easily re-orientate my models [preferably with batches of files]?

Thanks for your time!

 

[Timelord]

Browndoff,

I don't know of any way to fix old models, but for any new models, reset your view orientation in your templates so the "z" axis is facing out of the screen in the top view and the other views are the way you want them i.e. front and side views are oriented to the front and right planes.

Timelord

 

[Browndoff]

Thanks Timelord - but HOW do I 'reset the view orientation in the Templates'? Obviously one could rotate the view but then one must reset the 'system' somehow to make the change part of the template - how is THAT done?

BAC

 

[CorBlimeyLimey]

Does your clients' CAD import SolidWorks files (with features intact) or do you have to create a dumb (featureless) format?

 

[JMarv]

Open your model template, hit the spacebar to bring up the view orientation dialog. Orient the view to what you want to become the new "front" view. In the view orientation window, highlight "front" and then click the button for "update standard views." (It's the telescope with a clockwise rotating arrow around it, third button from the left.)

Joe
SW Office 2006 SP5.1
P4 3.0Ghz 1GB
ATI FireGL X1

 

[mjcole]

I'd suggest to use what JMArv told you but In my opinion your company should have done that before creating all your models. The Solid Works co-ordinate system is not a real co-ordinate system it's just used as that when exporting unless you create a co-ordinate system feature to be used when exporting.

If you use the reorient and update standard views option it will screw up all your current drawings. To permanantly fix your problem for future models open yor default Part and Assembly templates .prtdot and .asmdot files found in
C:\Documents and Settings\All Users\Application Data\SolidWorks\SolidWorks 2008\templates\ and mmodify those and save or save as to get new default templates.

Michael

 

[Browndoff]

Thanks, Guys!!!!!

I can't believe it's do straight-forward!! I have already modified all my Templates!

BAC

 

[CorBlimeyLimey]

Browndoff ... Be aware that the re-orientation method suggested is a non-permanent fix; any user opening the modified-orientation files can (at any time) just as easily reset the orientation using the Reset Standard Views button.

Also, the main Reference Planes will still refer to the original orientation ... but they can easily be renamed to conform.

Lastly, you should test whether your clients' CAD system recognises the new orientation. It may get lost in the export/import translations.

Which file format are you giving your client?
Which CAD system are they using?

 

[Browndoff]

Hi Guys,
Most of my clients use AutoCADand/or Inventor, so I export into *.igs - which, as I said before, left my part 'on edge' in their assemblies!

BAC