Converting Part view to 2D view 1

[Bhaveshn]

I have migrated from Solidedge.
How can I convert a part view to 2D entities which I can edit with 2D commands like trim, extend etc..

I don't care if it looses the association with 3D part.

 

[Eltron]

Are you looking to create a 2D drawing of your model? If so, go to File/Make Drawing from Part.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[Bhaveshn]

After making drawing, I want one view as non associated to Parent 3D part.

 

[CorBlimeyLimey]

Would saving as DXF or DWG suit your needs?

 

[CorBlimeyLimey]

Were you able to do as you describe in SolidEdge? If so what was that function called?

 

[Bhaveshn]

In SE, right click on view & select "Convert to 2D View" from pop-up menu

 

[CorBlimeyLimey]

If this function is important to you, submit an Enhancement Request (ER) at the Customer Portal.

https://customerportal.solidworks.c....swe?SWECmd=Login&SWEPL=1&SWETS=1267144948839

Can you give examples of why you use this function?

 

[PatCouture]

SolidWorks and Solid Edge are different when it comes to 2d drawings. Solid Edge will use the 3D model to generate a standalone 2d view of the model vs SolidWorks who will directly presents the 3d model as a 2d view. The difference may be subtle but for certain functionnality it makes a huge difference. For example SW needs to loads the 3D model in order to show the 2d view on the drawing if he doesn't have access to the .sldprt or .sldasm then nothing will show on the drawing. In SE the drawing is referenced to the 3d model but can still be viewed even if you don't have the 3d model available because the lines were generated at the time of the creation of the view.

Having said that, you won't find many 2d tools in the drawing package of solidworks because it's made that way. For my part I really miss this functionnality from my old days with SE.

So if you don't require to keep the associativity between the 3d model and the drawing views then as others suggested your best option is to export as .dwg and use Draftsight or other 2d software to do the editing.

Hope it helps

Patrick

 

[MadMango]

Read up on detached drawings in SW Help. I've never tried to make a single view detached, so not sure if that will work.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[Bhaveshn]

CorBlimeyLimey,

I want to quickly alter assmebly drawing to show better designs. I can always print & sketch over it but it won't be to scale & sometime confuse people in meeting. (crossing out line etc..)

It takes lot of time to change all parts in 3D to show various design enhancement options for existing assembly.

Hope this explains its use, if we have this in SW.

Bhavesh

 

[Bhaveshn]

Hi PatCouture,

I found workaround. export it to dwg, open dwg in SW. copy/paste required view back to original file.

It is not direct but not bad.

Thanks for help everybody.

Bhavesh

 

[fcsuper]

Bhavesh,

Have you considered saving the drawing as a Detached Drawing? This stores the 2D information and doesn't require the 3D model unless you wish to update (reattach) the drawing. To detach the drawing, goto File>Save As...> and select file type "Detached Drawing".

Also, you can log onto the SolidWorks Customer Portal website and goto the Enhancment Request area to find open requests for similar functionality for individual views. The more people that vote for those requests, the most important they become.

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion