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giovanni79
Posts: 8
Registered: ‎04-08-2009
Message 1 of 12 (2,390 Views)
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IDW vs DWG, what to use?

2390 Views, 11 Replies
12-14-2012 08:06 AM

Recently our company moved from SolidWorks to Autodesk Inventor (mostly because of the integration of the components of the Design Suite). Overall, the Inventor workflow is very similar to the one in SolidWorks and I find no significant difference between the two programs.

 

However, Autodesk Inventor offers the option to create drawings as IDW or DWG files. I would like to know why you would prefer one over the other one: everything I need to do seems to be doable in the IDW files. Are the DWG files present for compatibility with AutoCAD users only or are there other advantages? Is AutoCAD more flexible and thus it would be preferrable to do the drawings of Inventor parts in AutoCAD? What are the advantages of one format/workflow over the over one?

 

Thank you for your suggestions.

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Cadmanto
Posts: 3,191
Registered: ‎12-07-2011
Message 2 of 12 (2,387 Views)

Re: IDW vs DWG, what to use?

12-14-2012 08:12 AM in reply to: giovanni79

Oh, the more you use it the more differences you will find.  :smileyvery-happy:

 

The difference between .idw and .dwg is the .dwg is a more compatible format for Autocad directly out of

Inventor where as the .idw is a direct parametricly created drawing from Inventor.

 

Hope this makes sense to you.

Best Regards,
Scott McFadden
Inventor Professional 2013
(Colossians 3:23-25)

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giovanni79
Posts: 8
Registered: ‎04-08-2009
Message 3 of 12 (2,369 Views)

Re: IDW vs DWG, what to use?

12-14-2012 09:40 AM in reply to: Cadmanto

Thank for the comment. So it boils down only to compatibility with AutoCAD? Any advantage in using IDW?

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Curtis_Waguespack
Posts: 2,802
Registered: ‎03-08-2006
Message 4 of 12 (2,367 Views)

Re: IDW vs DWG, what to use?

12-14-2012 09:42 AM in reply to: giovanni79

Hi giovanni79,

 

For the most part they are the same with some differences here and there.

 

  • Are the DWG files present for compatibility with AutoCAD users only or are there other advantages?

It largely depends on the needs of your company. If you have then need to hand drawings to another department that uses only AutoCAD, then there might be an advantage to using an Inventor DWG. But you could also just Save off a copy of a IDW as an AutoCAD DWG or DXF, just as you might have done with SWx.

 

  • Is AutoCAD more flexible and thus it would be preferrable to do the drawings of Inventor parts in AutoCAD?

No, you'll be better off to detail the drawings in Inventor.

 

  • What are the advantages of one format/workflow over the over one?

* Inventor DWG file size is larger for the same drawing saved as an IDW

* You can use AutoCAD block in Inventor DWGs, but not IDWs.

* more mentioned below...

 

Autodesk Inventor supports IDW and DWG file types for drawings. Both file types produce identical drawings. IDW files are the native Inventor format. You can open them only in Inventor or Inventor View. This file type results in smaller file sizes.

The DWG file type is native to AutoCAD®. You can open DWG files in AutoCAD, Inventor, or DWG TrueView. If you create data using Inventor in a DWG file, you can modify the data only with Inventor. If you create data using AutoCAD in a DWG file, you can modify the data only with AutoCAD. If a downstream consumer of your Inventor data needs a DWG file, consider using DWG files as the default in Inventor.

 

Keep in mind that if a year from now you realize that one format or the other would work better than what you're using, you can batch convert the files to other file type using the Task Scheduler.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

 

 

 

 



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Cadmanto
Posts: 3,191
Registered: ‎12-07-2011
Message 5 of 12 (2,352 Views)

Re: IDW vs DWG, what to use?

12-14-2012 10:04 AM in reply to: giovanni79

The advantage of an IDW is that is the parametric drawing that is created right out of Inventor when you

place views from your model.  It is the direct drawing link to the model.

The IDW to Inventor is like the .slddrw in Solidworks.

Best Regards,
Scott McFadden
Inventor Professional 2013
(Colossians 3:23-25)

Valued Mentor
jclaidler
Posts: 512
Registered: ‎10-29-2009
Message 6 of 12 (2,345 Views)

Re: IDW vs DWG, what to use?

12-14-2012 10:14 AM in reply to: Cadmanto

The advantage of an IDW is that is the parametric drawing that is created right out of Inventor when you

place views from your model.  It is the direct drawing link to the model.

The IDW to Inventor is like the .slddrw in Solidworks.

 

Inventor DWG's are also parametrically linked to the models.

 

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PaulMunford
Posts: 898
Registered: ‎11-13-2006
Message 7 of 12 (2,239 Views)

Re: IDW vs DWG, what to use?

12-20-2012 11:46 AM in reply to: giovanni79
DWG s are handy if you are using g AutoCAD and Inventor. Both AutoCAD and Inventor views can be combined in one file. Inventor doesn't have a sheet set manager - AutoCAD does. I guess IDW is better if you are purely Inventor...
The CAD Setter Out Blog @CadSetterOut

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rjezuit
Posts: 35
Registered: ‎03-09-2011
Message 8 of 12 (2,231 Views)

Re: IDW vs DWG, what to use?

12-20-2012 12:45 PM in reply to: PaulMunford

We use Inventor and ACAD. We use .idw's for Inventor and .dwg files for ACAD. This shows instantly whether the drawing is a parametrically linked file to a part or assembly, or a 2D generation from ACAD just by looking at the file extension. Just something we found handy.

Valued Contributor
DVDM
Posts: 112
Registered: ‎09-24-2009
Message 9 of 12 (2,207 Views)

Re: IDW vs DWG, what to use?

12-20-2012 04:00 PM in reply to: rjezuit

Many users would be hard pressed to spot the difference between an idw and an Inventor dwg file while editing in Inventor.

I've decided on making Inventor dwg as the standard. Yes the file is somewhat bigger in size because every view is stored as an autocad block, but the benefits outweigh that.

 

For example, I have a drawing of a huge assembly, thousands of parts. An engineer wants to have a look at the drawing, measure up a few things, etc.

With Inventor idw, he/she would open up that drawing in Inventor, which would then try to load the entire dataset into memory, worth 100's of MB, taking ages and potentially a whole bunch of missing file references and intimidating warnings along the way.

With Inventor dwg, he/she would open a single file worth just a few MB's in AutoCAD, which is an exact representation of the model in its last saved state, which would open very quickly, and can be navigated and measured in with ease.

 

Because we still have a mixed setup with top level assemblies in 2D AutoCAD, but parts/subassemblies in Inventor, up-to-date blocks of these Inventor components can be quickly inserted into the 2D AutoCAD file. These blocks can even be kept up to date with the help of Design Centre, though admittedly this is not the smoothest of workflows.

 

Contributor
robbeckley
Posts: 18
Registered: ‎12-06-2006
Message 10 of 12 (2,187 Views)

Re: IDW vs DWG, what to use?

12-21-2012 01:59 AM in reply to: DVDM

Interesting that it has been mentioned at least twice that the file size is larger for DWG,  I have done  a lot of comparisons and have found consistently that DWG file size is smaller….

 

However I concede that will depend on the typical way in which you represent your engineering drawings, if the drawing is a plain line drawing with no colour graphics the file size is less than half typ 2.4 mb IDW to 0.9mb DWG, as soon as you add textures colours the opposite (ish) happens 2.4mb IDW to 3.8mb DWG.  Presumably the graphic information is stored as a raster image in the AutoCAD file which would make the file a lot larger than purely vector information.

 

-edit - on larger assemblies with sufficient vector information this scale can tip and the DWG’s will become larger, my survey was based on smaller part drawings.   

 

I would like to hear views to back up this for or aginst of course this is just my sumamising based on the drawings I have had available.

 

One of the main reasons I have for using DWG’s is you can use any DWG viewer /Compatible CAD programme to view the drawings, which would mean not having to use Inventor View! Which has the odd teething trouble when installing every year.

Rob B.

Win7 64 Pro - Asus P8P67 PRO - i5-2500k CPU O/C@4.5Ghz- OCZ Vertex 2 SSD - 8GB Ram - GTX550 Ti - SpaceExplorer.

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