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new perspective at Solid Works
2

new perspective at Solid Works

new perspective at Solid Works

(OP)
I would like to know if I can add a extra perspective at Solid Works. You've got already Isometric,Trimetric en Dimetric, but I would like to add the next perspective: from left to right 30 degre,90 gdegre,60 degre

How can I add this perspective?

RE: new perspective at Solid Works

SanRox,
You can add any view you like to each model.
Orient the model the way you want, Go to standard view toolbar, view orientation, and name the new view there.
Then, when you get to your drawing, you can place the view with the newly saved orientation.

I have a feeling by the way you ask that you want the view always available.  Perhaps other heavy hitters know how to achieve this.

regards,
dsgnr1

¿)

At some point you just have to shoot the engineer and build the dang thing.

RE: new perspective at Solid Works

(OP)
So can anyone help me?

RE: new perspective at Solid Works

(OP)
and I want the view always available

RE: new perspective at Solid Works

SanRox,

You can achieve your view the way dsgnr1 describes.  You will need to manually rotate your model into the desired orientation and save that view orientation so it can be re-used.  If you want to have this view available in evey model you will need to create a macro that automatically creates the view orientation you are looking for.  Once you create a new model you run the macro and the view orientation will be added.

Rob Rodriguez CSWP
www.robrodriguez.com
SW 2006 SP 1.0EV

RE: new perspective at Solid Works

(OP)
But how do I know that the middle section is exactly 90 degre. Is there no function to lett the program calculate this?

RE: new perspective at Solid Works

There is a macro freely available that creates 8 isometric views. By searching this forum or searching the net you could find that macro and modify it as you want.If you are unable to find the macro let me know and I will find a way to send it to you.

RE: new perspective at Solid Works

Custom views do get stored in templates, so if you make a new assemby, create the required views and save it as your new default assembly you won't even have to use the macro on new designs.

Stefan Hamminga
Mesken BV
2005 Certified SolidWorks Professional
Mechanical designer/AI student

RE: new perspective at Solid Works

Welcome to the forum SanRox...
Looks like you owe a star to StefanHamminga

Good catch Stefen!

regards,

dsgnr1

¿)

At some point you just have to shoot the engineer and build the dang thing.

RE: new perspective at Solid Works

(OP)
@ netshop21 can you please sent me the macro, I can find anything and I don't know how it works

RE: new perspective at Solid Works

(OP)
keej thanx I hope this topics will help me

RE: new perspective at Solid Works

(OP)
the macro of the IsoViews doesn't work with Solid Works 2005

RE: new perspective at Solid Works

This may seem stupid, but I just set me arrow keys up to a certain degree in the system options menu and then use my arrow keys to set the model in a perspective that I want. Click the Spacebar, click middle telescope and save the new view and use that new view in my drawings.

Maybe old school but that's just me I suppose.

Regards,

Scott Baugh, CSWP
www.scottjbaugh.com
FAQ731-376

RE: new perspective at Solid Works

Matt Lombard offers some macros for additional views on his web site, http://mysite.verizon.net/mjlombard/ I've not used them so I do not know if they are what you are looking for. Hope it helps.

RE: new perspective at Solid Works

I do the same thing Scott.

"I think there is a world market for maybe five computers."
Thomas Watson, chairman of IBM, 1943.
Have you read FAQ731-376 to make the best use of Eng-Tips Forums?

RE: new perspective at Solid Works

As do I--arrow keys by default move the "perspective" of your viewport by 15 degrees--works great with what is discussed in this thread.

Add the views to a template and they will be "permanent", as Stefan mentioned.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: new perspective at Solid Works

It worked great in SW2003. I updated my templates using the "IsoViews - All 8 of them   FAQ559-529" macro back then & have used those templates ever since. I guess the SW05 macro "calls" (?) must have changed.


Helpful SW websites  FAQ559-520
How to get answers to your SW questions  FAQ559-1091

RE: new perspective at Solid Works

Sanrox,

I updated the macro for my own use to work in SWx2005

Sub main()

Set swApp = CreateObject("SldWorks.Application")

Set Part = swApp.ActiveDoc

pi = 4 * Atn(1)
Z = Tan(30 * pi / 180)
X = Atn(Z / Sqr(-Z * Z + 1))
Y = -45 * pi / 180

Part.DeleteNamedView "TRF-ISO"
Part.DeleteNamedView "TRR-ISO"
Part.DeleteNamedView "TLF-ISO"
Part.DeleteNamedView "TLR-ISO"

Part.DeleteNamedView "BRF-ISO"
Part.DeleteNamedView "BRR-ISO"
Part.DeleteNamedView "BLF-ISO"
Part.DeleteNamedView "BLR-ISO"


Part.ShowNamedView2 "*Front", -1
Part.ActiveView().RotateAboutCenter X, Y
Part.ViewZoomtofit
Part.NameView "TRF-ISO"

Part.ShowNamedView2 "*Right", -1
Part.ActiveView().RotateAboutCenter X, Y
Part.ViewZoomtofit
Part.NameView "TRR-ISO"

Part.ShowNamedView2 "*Back", -1
Part.ActiveView().RotateAboutCenter X, Y
Part.ViewZoomtofit
Part.NameView "TLR-ISO"

Part.ShowNamedView2 "*Left", -1
Part.ActiveView().RotateAboutCenter X, Y
Part.ViewZoomtofit
Part.NameView "TLF-ISO"


Part.ShowNamedView2 "*Front", -1
Part.ActiveView().RotateAboutCenter -X, Y
Part.ViewZoomtofit
Part.NameView "BRF-ISO"

Part.ShowNamedView2 "*Right", -1
Part.ActiveView().RotateAboutCenter -X, Y
Part.ViewZoomtofit
Part.NameView "BRR-ISO"

Part.ShowNamedView2 "*Back", -1
Part.ActiveView().RotateAboutCenter -X, Y
Part.ViewZoomtofit
Part.NameView "BLR-ISO"

Part.ShowNamedView2 "*Left", -1
Part.ActiveView().RotateAboutCenter -X, Y
Part.ViewZoomtofit
Part.NameView "BLF-ISO"

Set Part = Nothing
Set swApp = Nothing

Set swApp = Application.SldWorks
End Sub

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford



 

RE: new perspective at Solid Works

Dang it, I forgot about CBL's FAQ on uploading files.  here is the link to the file.

http://www.mooload.com/file.php?file=files/1130869558/ISO_Views.swp

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford



 

RE: new perspective at Solid Works

Heckler ... The author of the original FAQ (StarrRider) does not appear to be active in the forums (since 2004-01-06 anyway), so perhaps you should post a new FAQ for the updated macro.


Helpful SW websites  FAQ559-520
How to get answers to your SW questions  FAQ559-1091

RE: new perspective at Solid Works

Scott, MadMango, Theo ... A small point, but using the arrow rotation method will not give true Isometric perspective views. Compound angles come into play.

Select the SW Isometric view of a part & then try to get back to a regular planar view, using the arrows, to see what I mean.


Helpful SW websites  FAQ559-520
How to get answers to your SW questions  FAQ559-1091

RE: new perspective at Solid Works

I also store predefined views in my drawing template. One is called "TitleBlock" and is very easy to get to from the tool bar or a macro.

--
Hardie "Crashj" Johnson

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