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Model Orientation

Question asked by Joel Nelson on May 29, 2011
Latest reply on Mar 13, 2012 by Jeremiah Feist

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I see that this question has been asked before from people like myself who are PRO/E users, trying to learn SolidWorks, so I appolgize for asking again. However, I feel that either I am not finding a answer that works, or is way to over complicated.

I need to create Isometric view for exploded assembly drawings.

Most of the previous post appear to state just orient the view till it looks good, and save that orientation.

Sorry, that is not good enough for me.

I am required by standard (company and customer) that isometric orientation be at a specific rotational value (45/35.26/30).

For example, from PRO/E I can orient a model in a Right Side view, and change the rotation by the values above, then save that new view for reuse.

The dialog box for this looks like this:

So my question is:

If I am oriented in a normal (right) view, is there a way in SolidWorks to create a Isometric view that is rotated in the H (45), V (35.26), C (30)?

Thanks in advance for any help

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Scott McFadden May 29, 2011 6:22 PM
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Hi Joel,
If you hit the space bar you will see all of your current view as out of the box.
When I personally do my exploded views I just spin the model in the view that works
for me, hit the space bar and at the top is a selection to save that view. You can also use the arrow
keys to change the view rotation as well.

http://help.solidworks.com/2011/english/SolidWorks/sldworks/LegacyHelp/Sldworks/Display/HIDD_SELECT_NAMED_VIEW.htm
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Wayne Tiffany May 29, 2011 11:46 PM
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The only quick way I can think of is to do it with a macro, and tie that to a hotkey if you wish. I have attached one of the macros that I use as part of the set that is tied to the number keypad keys. The number 9 key will create and rotate you to an upper right isometric view. If that's not what you want, you should be able to modify the numbers in the macro to get what you want.

The rest of the set goes to the other iso views and the front, left, etc. views. Very handy - I use them all the time. If you want to look at the whole set, go to KCSWUG.com and grab the keypad macros file.

WT
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- Num9.swp.zip4.7 KB
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Kelvin Lamport May 30, 2011 12:29 PM
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That might be a handy function to have in SolidWorks. I suggest you submit an ER (Enhancement Request) via the Customer Portal.

Meantime, you could use a macro as suggested, or you could import a Pro/E file which was set and saved at the required angle; Use the Orientation tool (Spacebar) to save the imported view; Delete all geometry to leave only the basic Feature Manager, and then save the empty document as a template. This way any new models will have the special viewing angle available via the Orientation toolbar.
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Alin Vargatu May 30, 2011 3:15 PM
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Let me propose 2 workarounds:

1. a) In the drawing, insert a model view.
b)From this view, create projected views at about 45 degrees - see below:

2. a) Create a camera with the desired orientation. Perspective Off, Target = origin.

b) Make that camera view active.
c) Save that view.
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- Mike Price @ Alin Vargatu on Oct 6, 2011 12:02 PM
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  Hi Alin,
  
  Just was looking for something about reorienting vies and came across this. I don't know exactly what you did to create a camera in the drawing and then show that in the model, if that's what you did.
  
  Joel's original question is one I've always just worked around in SW, but I'm tired of doing the work around and started doing some digging. I am able to get a model oriented just like I want in a drawing by using the Align Drawing View and then using an edge to make it horizontal (after I have made a view that is normal to a surface). I don't know how to do this in the model, but it seems that you are suggesting a way to do it......
  
  Thanks,
  
  Mike
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  - Deepak Gupta @ Mike Price on Oct 6, 2011 12:35 PM
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    Mike you can create a new view orientation at part/assembly level and then use that in the drawing as required view.
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    - Mike Price @ Deepak Gupta on Oct 6, 2011 1:18 PM
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      Just to clarify things a bit. This is the situation I have. I did a view normal to a flat surface. Now because of original geometry, the part is oriented as shown. I want to have the other edges perfectly horizontal/vertical (It is not at a 20 deg exact angle where I can manually rotate around, knowing it will be exactly lined up) In ProE, I can use one of the planes to get it to line up such that the edges are exactly horizontal/vertical. Again, it looks like Alin is suggesting that you can take a drawing view and then create a model view with the same orientation. I could then reassign all of the standard views based upon the drawing view........
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      - Deepak Gupta @ Mike Price on Oct 6, 2011 1:31 PM
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        Mike Price wrote:
        
        Again, it looks like Alin is suggesting that you can take a drawing view and then create a model view with the same orientation. I could then reassign all of the standard views based upon the drawing view........
        
        No you can't do that and neither he is suggesting this. He is showing two different ways of model orientation.
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      - Jeremiah Feist @ Mike Price on Oct 6, 2011 1:44 PM
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        you can (control) select a second face before activating the normal to comand. SW will use the second face as "up".
        
        http://help.solidworks.com/2011/English/SolidWorks/sldworks/LegacyHelp/Sldworks/Display/HIDD_SELECT_NAMED_VIEW.htm?id=59ee763558be4cf1aa4c8796bb345756#Pg0
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        Mike Price @ Jeremiah Feist on Oct 6, 2011 1:46 PM
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        After all this time...............
        
        Thanks Jeremy. That's very nice.
        
        Sorry all for hijacking the post, but as Deepak pointed out, I needed read Alin's post again as I was reading it incorrectly..........
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- Greg Van Arsdale @ Alin Vargatu on Oct 7, 2011 12:23 PM
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  Hello All,
  Forgive me for the digression, but since we switched to 2011, I can no longer get the view Orientation dialog to display.
  I assumed that it was discontinued in favor of the camera function. Does anyone know of a trick to show the view Orientation dialog?
  Is this a known bug? Thanks in advance.
  Enjoy this day,
  Greg
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  - Deepak Gupta @ Greg Van Arsdale on Oct 7, 2011 12:30 PM
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    Try any of these to get the dialog box or options:
    
    Click View Orientation (Heads-up View toolbar), and select a view orientation.
    Click a view orientation on the Standard Views toolbar.
    Press Spacebar (a shortcut key)
    View > Modify > Orientation
    
    In case you still get it, then it might have moved out of the SolidWorks window or possibly got corrupted.
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    - Greg Van Arsdale @ Deepak Gupta on Oct 7, 2011 1:12 PM
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      Hi Deepak,
      The pull down menu indicates that it is displayed.
      Maybe it is displayed beyond the limits of my screen's bezel.
      Or it might be a gremlin associated with my dual display set up.
      That's life I guess!
      Thanks!
      Greg
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      - Deepak Gupta @ Greg Van Arsdale on Oct 7, 2011 1:15 PM
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        Try changing you screen resolution or decrease the SolidWorks window size and once you find it, you can drag it back inside.
        
        OR
        
        The another way might be to fix it up via some registry settings.
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        Greg Van Arsdale @ Deepak Gupta on Oct 7, 2011 2:22 PM
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        Hi Deepak,
        I tried your first suggestion to no avail.
        I leave the registry alone for fear of upsetting the IT folks.
        Thanks for all your suggestions!
        Have a super weekend!
        Greg
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Erik Bilello Oct 6, 2011 5:08 PM
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Joel,

A construction plane can be precisely oriented relative to the default planes. Create a plane normal to each view orientation you need. Use these planes to make Named Views. Save templates of course. You can delete the construction planes without losing the Named View orientation. The view orientation is not linked to the plane.
A bit of a pain for the stuff you already have done, but once you have templates with your required views it should be as easy as using the current defaults.
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- Marshall Long @ Erik Bilello on Oct 7, 2011 12:31 PM
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  try mating your part to a reference plane. This will flip the hole part to exactly where you want it.
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  - Erik Bilello @ Marshall Long on Oct 7, 2011 7:23 PM
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    Marshall,
    
    I'm assuming from his post that Joel probably needs to keep his parts and assemblies aligned with the Front,Top and Right planes to meet the standards of company and customer. So, he needs a way to get an exact viewing angle relative to these default planes. As I state earlier it seems fiddely at first, but once you have a template you're all set.
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Mitch Gilbert Mar 13, 2012 2:43 PM
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Hello,
I'm also a ProE guy who has migrated to Solidworks & the view orientation that only allows one selection is a headache, however, what I do is measure the angle of the 2nd surface you wish to orient (with respect to some original plane) then set your view rotation increment (System Options - view) with the arrow keys to be some fraction of the desired rotation. Then use the arrow keys to orient the second surface & save the orientation using the space bar etc (you can reset your arrow key increment after your done).
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- Jeremiah Feist @ Mitch Gilbert on Mar 13, 2012 2:50 PM
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  See this post
  https://forum.solidworks.com/message/251516#251516
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