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SeanFarr
Posts: 475
Registered: ‎07-25-2012
Message 1 of 7 (539 Views)
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View Reps or LOD's?

539 Views, 6 Replies
01-17-2013 07:02 AM

I have created all my individual part detail drawings for a project and am now ready to create GA drawings. Instead of creating many assembly to show how groups of parts are assembled and added to the main assembly. I understand that I can create View Reps and LOD's. I have been reading up on them and the only difference that I can come up with is, VR turn off visibility and LOD suppresses parts. Having no experience with this, I can't make a decision as to what I need or is best?

 

I have a frame structure with sheet metal parts to enclose it. So basically my approach was to assemble in section, Front, Left, Back, Right and Top. (see image). I can create a VR or LOD for each and then detail that in my drawings.

 

Any suggestions?

 

Thanks

 

Sean Farr

 

Inventor Pro 2013

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Valued Mentor
SeanFarr
Posts: 475
Registered: ‎07-25-2012
Message 2 of 7 (529 Views)

Re: View Reps or LOD's?

01-17-2013 07:28 AM in reply to: SeanFarr

I just drove home and grabbed my Mastering Autodesk Inventor 2012 book, and have read the chapter on Representations. It seems the major difference between the VR and LOD's is that LOD's suppress parts/assemblies which means less RAM is required. Very helpful for large assemblies. For my assembly, less than 200 basic parts, VR should be more than adequate.

 

I didn't find anything that talks about how the two separate representations correlate to each other. Is there things to watch for, say having a LOD of a particular VR? or is this common practice? Use one or the other?

 

Thanks


Sean

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
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Curtis_Waguespack
Posts: 2,828
Registered: ‎03-08-2006
Message 3 of 7 (525 Views)

Re: View Reps or LOD's?

01-17-2013 07:36 AM in reply to: SeanFarr

Hi SeanFarr,

 

Keep in mind that you can create an LOD and then right-click on it and choose Copy to View Rep or create the View Rep first and copy to an LOD, so the two are pretty flexible and can indeed be used together. But they do have different purposes as you've mentioned.

 

An important question for your situation though, is how you expect your BOM to look?

 

If I understand correctly, you've created a configurable assembly and intend to create a representation (LOD or View Rep) for each configuration. If that is the case, then I think what you really want are iAssemblies, as they will hand the BOM configurations correctly.

 

You'll struggle to get a correct BOM with View Reps (you'd have to use Parts List filters), and you will not be able to get LODs to give you a correct parts list.

 

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



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Valued Mentor
SeanFarr
Posts: 475
Registered: ‎07-25-2012
Message 4 of 7 (513 Views)

Re: View Reps or LOD's?

01-17-2013 07:57 AM in reply to: Curtis_Waguespack

I suppose I shall have to experiment to see what exactly comes out in the BOM.

 

What I am expecting, is the view(VR or LOD) of the drawing, to list those parts only and not the entire assembly in the BOM. As you have said, filters may be needed.

 


If I understand correctly, you've created a configurable assembly and intend to create a representation (LOD or View Rep) for each configuration. If that is the case, then I think what you really want are iAssemblies, as they will hand the BOM configurations correctly.

My assembly is more 'adjustable' than configurable in a sense. The assembly will always have the same parts in the same locations, just the overall size changes. The current assembly is the smallest size, roughly L-9'xW-4'xH-5' and our biggest so far is L-12'xW-5'xH-6'. So not much different. Just lengths and widths get changed. 

 

Does this make a difference about anything? I am making a 'base' package and for each project from now on, I would use the design copy tool, create a new project, adjust the assembly and was hoping that all drawings would update accordingly. They would of course need reviewing to ensure that all views were still on the drawings and not extended off and that dimensions are not overlapping or on top of one another.


If size changes to the assembly are done? does the VR or LOD update as well?

 

I am not under critical deadlines at the moment, so I will investigate iAssemblies this afternoon.

 

Thanks!!

 

Sean Farr

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
*Expert Elite*
Curtis_Waguespack
Posts: 2,828
Registered: ‎03-08-2006
Message 5 of 7 (503 Views)

Re: View Reps or LOD's?

01-17-2013 08:22 AM in reply to: SeanFarr

Hi SeanFarr,

 

Ok, I think I understand now. You're wanting to use Representations instead of subassemblies, so that you can show the assembly in stages as it's built.

 

I think View Representations are the way to go then, as you can filter the parts list by View Rep. Just be aware that some QTYs may need to be adjusted. For instance, you have 3 of the same part number in your assembly, and you only show 1 in your View Rep, your parts list (even when filtered to look at the View Rep) will still show the total QTY of 3. So it's kind of an all or nothing situation.

 

If that's going to trip you up, then iAssemblies might be the way to go, otherwise View Reps should work fine.

 

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

 

 



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cwhetten
Posts: 1,054
Registered: ‎09-03-2008
Message 6 of 7 (499 Views)

Re: View Reps or LOD's?

01-17-2013 08:39 AM in reply to: SeanFarr

We have a rather complex assembly that we have set up to change configuration in many ways.  It uses iLogic heavily, doing a lot of component replacement and suppression, as well as changing parameters to adjust the sizes of parts.

 

As I mentioned, we chose to go with suppressing components (which requires a custom LOD).  We did this because we noticed that when suppressing components with iLogic (using the Component.IsActive( ) function), these components were automatically removed from the bill of materials, making our parts list lines and quantities display correctly.

 

It works quite well.  However, there are some issues with using custom LOD's that will undoubtedly frustrate you.  When working on a drawing of an assembly with a custom LOD, if you also have the assembly open, sometimes Inventor will refuse to save the documents.  The workaround is to close one or the other document, or to never have them open at the same time.

 

Also, sometimes in an assembly with a custom LOD, Inventor will refuse to open the BOM editor.  Inventor will toss up a message box saying something about needing to save the document first, but no matter how many times you press the save button, it will still keep saying this.  Usually, after rebuilding a few times and saving and closing and re-opening and saving and closing and re-opening again and again and again, Inventor MIGHT open the BOM.

 

In light of these frustrations, we have decided to try using view reps for our next project to see if we can get away from using custom LOD's entirely.  In order to get the BOM lines and quantities to display correctly, we have to add an extra line of iLogic code to turn the component's BOM structure to Reference when its visibility is turned off.  So far it is working well, but we are just in the preliminary stages of development; as such, I can't fully recommend this method yet.

 

-cwhetten

Please click "Accept as Solution" if this response answers your question.

Valued Mentor
SeanFarr
Posts: 475
Registered: ‎07-25-2012
Message 7 of 7 (493 Views)

Re: View Reps or LOD's?

01-17-2013 09:05 AM in reply to: Curtis_Waguespack

Yea, I should have written what I was trying to do explicitly in the first post to clarify my questions.Thanks Curtis, for you guidance, I should be able to handle the QTY issue as I will probably have less than 10 unique parts per view. 

 

I appreciate your input as well cwhetten, all info is helpful and I will most definitely be looking into this down the road, however, I am fairly new to programming/iLogic, so I'm taking baby steps with it trying to understand. I know Inventor makes it easy to use, but it is still a new language to me. The syntax is the troublesome part, knowing what statements to use and what each function is and does. But nevertheless, all in time it will come together.

 

I love this forum!!!

 

Thanks again, have a good day..

 

Sean Farr

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49

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