Component Isolation for Drawings

[Anonymous]

Hi, 

I have a pretty large and adaptable assembly through iLogic. I am trying to make shop drawings for each component to be fabricated by our welders. what I started to do  was open a certain view of the entire assembly, and then turn the visibility off of everything I didn't need. This is time consuming, and as my assembly changes in size through iLogic, the drawing seems to add peices that I need to go back and turn off. 

I read another post about creating view representations but this also seems time consuming. Could the best way be to simply create a drawing based off the specific components part or assembly file? I feel like doing that is like skipping a step. There has to be a better way to do this. 

I am using Inventor 2016 with vault basic on windows 7 prof, 64 bit..

Any help is greatly appreciated, 

Thanks

Sandro

[CCarreiras · Accepted solution]

Hi!

Better and secure way is using View Representations Locked.

True, at beginnig you will take some time to make all that View Repr. you need, but when finished and locked, you will never have to do it again.

Tips:

• Create the View representation with the master Level of detail.
• You can use the view representation as a filter of part list
• Make the view repr. at final stages of the assembly. When you insert a new part (i'm not speaking about suppress/unsupress), sometimes it can appear in some levels of details unlocked, you have to unlock, correct and lock again.

[Anonymous]

I've ran into this same issue or something close to it.  I ended up bringing individual parts/sub-assys into my main drawings to make the details.   I do this so I can pull part number/description/mat'l through into the view label for purchasing.  (note: Item number reletive to the main assy will not work)  I used to run view reps that were locked and they worked fine but bringing individual parts is faster and allows me to link BOM info into view label. 

[blair]

I would go with "ccarreiras" method of creating View-Reps within your IAM as well. You can isolate the item you need my suppressing all the other components.

Normally we go with the single part-single drawing methodology. Should something happen to corrupt either your parent IAM file of IDW, you don't loose all your work.

The main drawing for the IAM should only contain information that pertains to the main IAM file. Any sub assemblies should be detailed by them selves and the same for any single IPT files that require a drawing for their creation.

If you need to put together a "drawing package", export each drawing to a PDF and use other software such as Adobe Acrobat to combine the individual PDF's into a single PDF file.

[Anonymous]

I really appreciate the responses guys. I still have questions.  

What I am currently attempting to do IS create a drawing package. I have my first drawing of the entire assembly, then a series of component drawings for the welders to use. I am creating a new sheet for each component within the drawing file which by the sounds of "blair's" last post, doesnt seem to be the best way to do this? Am i reading this correctly?

[CCarreiras]

HI...

Really there's no rule....  it deppends...but...

In my systems i used to do this:

I Have a drawing document for the main assembly... this doc lauch other documents:

I have a drawing document for each "Main Assembly's part"

I have a drawing document for each "Sub Assembly": first sheet Assembly, and other sheets, one sheet for each "sub-assembly's part"

Check your private message box...

[rhasell]

Hi

All I can add besides what has been mentioned:

Please do not use multi sheet drawings.

Create a drawing for each assembly/sub assembly/part.

Rule of thumb:

If you need to create a new sheet, then STOP... create a new drawing file.

If you need the sheet counter (Sheet 3 of 10) then create empty sheets, edit them them to exclude them from printing.

Reasoning:

1: If something gets damaged or corrupted, you only loose one drawing.

2: Have you seen how big these files get? can you imagine tying to work with a drawing file approaching 10's to 100's of megs in size?

[Anonymous]

Hi again,

ok, so I am putting my trial and error process on hold until I really have this understood.
So for every single drawing I want to create, I should have a whole separate drawing file? Inventors use of "sheets" is basically useless? I was very happy to see the sheet counter as renumbering title blocks manually in AutoCAD LT is incredibly cumbersome.
If this is the best way then I guess I will just have to accept it. When creating these entirely new drawing files, should I always be starting with the top level assembly and then using a view rep? I have tried creating a drawing that referencing just the part file that I want to see but when I made a change in iLogic, all annotations had broken links...

I really appreciate the help guys, once again i really didnt realize something that I thought would be so simple has turned into something so complicated.

Thanks
Sandro

[Anonymous]

just a bit to add to this...I tried making the view rep for one part now, and it seemed to be a pretty good way to do it. It was time consuming but not as bad as i expected.

My problem is that Inventor really doesnt seem to be intelligent enough while using iLogic. I made my assembly bigger which then added some parts or added holes etc...These new parts showed up on the drawing AND some of my annotations were no longer linked to their proper holes (to show spacing)

I cant be the first person to do this...I would really appreciate some assistance! Thanks again!

Thanks
Sandro

[blair]

You will need to suppress them in the model browser. Inventor doesn't know if you want them in that view-rep or not, so them come in visible in all view-reps until you suppress them in each view-rep

[Anonymous]

blair,

I tried that and it appeared that when I suppress a part, it suppresses it in all view reps. only turning the visibility off seemed to give me the results im looking for. Am i doing something wrong?

Thanks
Sandro

[blair]

Sounds like you missed the part of Suppressing in each View-Rep that you don't want to see the part. If you Suppress the part in the Master View, then it will be Suppressed in each View Rep.

You need to activate each View-Rep and Suppress the part in each view.

[Anonymous]

Hi Blair,

I have tried what you have said in multiple ways. I Have created a couple of different view reps. while the new view reps are active, suppressing a part within that view rep is also suppressing it in all other view reps including the master. My drawings will not work this way.
This is only adding to the issue that when new parts are introduced with iLogic because of patterns, they appear on my drawings (not in view rep?) even when i have that patterns visibility turned off...

[blair]

I've never seen this behaviour, it's always worked for me and the others that have suggested this method. I don't have time to do a ScreenCast showing this method this week as I have a number of things to get done before I head to AU next week.

If you created a ScreenCast (ADSK software) of the method you are using, we should be able to solve this for you.

[Anonymous]

I am sure this method works, but as with everything else I ever try to do with this program there is something I am doing fundamentally wrong.
I have never made a screencast so im going to have to just try to explain.

I have a master assembly which is adaptable by iLogic. I am using the "default" View Representation with a custom "Level of Detail." I am pretty sure this is the norm..

All i did was right-click on the "view" tree and click "new." From that new view rep I turned the visibility off of everything i didnt need to see for the purposes of that specific drawing. I then opened a drawing file and made one sheet for the top level assembly, and one sheet for the "part"

When choosing the base view for the "part" I selected the new view rep I had created for it. All other problems I encountered have been stated in my earlier messages.

Could this have something to do with the Level of Detail? Keep in mind I am still relatively new with Inventor..

Thanks
Sandro

[blair]

Did this quickly in the LOD, the view can be copied to the View Rep as well. If I add a new part, it will be active in all View-Reps and LOD's. I would have to enter the desired View and Suppress the part, then do a Save to save the updates.

http://autode.sk/1Xlj63M

[Anonymous]

That was great! thanks blair.

I really thought this was going to be the answer. Previously I was not doing anything with the Level of Detail. I was only creating a new View.
This time i followed your steps and everything you said earlier made sense and worked correctly. I could suppress parts in one level of detail and they would still be there in another. Unfortunately this did not solve my iLogic issue. Whenever patterns in the assembly generate another part, the part shows up in the drawing AND NOW the Level of detail...even when the pattern is suppressed!!

This is so frustrating. I really appreciate your help!

Thanks
Sandro

[CadUser46]

bnwtech.  We create multi-sheet multi-item drawings all the time.  In 10 years i have seen maybe 1 or two get corrupted.  In PDM/ERP having each member as its own file/partnumber represents its own object so this would be be many many more objects that need checked and approved with each cycle.

We on the other hand get around this problem another way.  Its still not perfect but saves you needing to create reps for each member in each weldment and overall the pro's outweigh the con's.

We have two VBA routines.  We place a view of the whole weldment then using part priortiy the first routine turns off every member expect the one the user selected.  The second routine is for re-hiding everything that has appeared since the views were placed.

If you do go down the single sheet drawing route you should look into other automation tools that collate the pdfs/dwfs automatically for work prep.

Blair.  What do you use to make that screencast?

[Anonymous]

Hi again,

sorry I am pretty new to Inventor and have absolutely no experience with VBA so this solution is not very well suited for me unfortunately.

I am getting increasingly frustrated with this problem. I can not believe that simply creating drawings of my model is becoming so difficult.

How are suppressed patterns still generating parts? How come my view and LOD shows only the part i want to create a drawing of, but the actual drawing is showing parts i cant even see on the model?! I am sure iLogic is the culprit of this and the makers of Inventor haven't worked out all the bugs but I find it very hard to beleive that nobody has tried to make drawings of an iLogic adaptable assembly...

[CCarreiras]

HI!

There's no bug at all...

The question is, when you create the views, you have to select the same view representation and the same Level of detail as the ones you have in the assembly!!!