View Orientation 1

[halfmark]

In the SW 2004 I would be able to select a surface in a part model or assembly, and choose normal to. I would then drag that view onto a drawing sheet. Now it seems my drawing view orientations are limited to top, bottom, right side etc etc or I have to use the rotate view comand. There are situations where I find it necessary to manualy orient a model to show specific detail information. My question is this: is there a way for me to manualy orient my view in the model , and then place it in a drawing and keep that orientation.

Mark R.G. RAY Clamps corp.

 

[J-C]

1. Get the view orientation you want, hit teh space bar and save the save teh view to the list.

or..

2. Orient the view in the model, go to the drawing, insert a new drawing view and select "current".

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP0.0 on WinXP SP2

 

[halfmark]

Thanks That did the trick!!!!!!

Mark

 

[yanceman]

Halfmark,

Here's one you probably won't find in the SW books. After selecting the model face that you want to view normal to, hold the control key and select a face that is 90° to that face and then click the normal to button. The face that you selected 2nd will orient upwards like a top view. Try this a few times. It's pretty cool.

Jeff

 

[wes616]

Insert > Drawing View > Relative to Model

It puts you into the model, and you can select 2 surfaces to orient the model from....

This is handier than the current view, because you can edit the model w/o the drawing view moving.



Wes C.
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There are no engineers in the hottest parts of hell, because the existence of a 'hottest part' implies a temperature difference, and any marginally competent engineer would immediately use this to run a heat engine and make some other part of hell comfortably cool. This is obviously impossible.