I need help with exploded views and separate part numbers on drawing

[technologybuskirk]

I'll try to explain in the best way I know how what we did. We are trying to create IDW files for our manufacturing floor AND use them to help create a manual and assembly instructions for customers. I created a presentation, I blew them all up, and did everything to where we would like it. Then I created the IDW and everything seemed great. I wanted to reflect a part list to show what parts they would work on in every sheet of the IDW. Only showing what they are working with. I thought I could do this with the filter ballooned items only. The problem was they reflected the balloons on every sheet. I've been trying to figure this out all day trying different things I've read here or there. There has to be a way to create the presentation snapshot views and have a corresponding list of parts for each page that will update if/when we update a part. How would I achieve this?

[LT.Rusty]

I believe you might be overthinking the problem.

Insert your .IPN view into the drawing as you normally would on each page, and insert the parts list. Then right-click on your parts list table and select "EDIT PARTS LIST" (not "BILL OF MATERIALS"). You can set the visibility for each line of the parts list from here- right-click on the line you want to turn on or off, then click "VISIBLE" to check / uncheck it.

This will give you per-sheet visibility on the parts list items, but unfortunately it won't let you renumber the parts on each sheet. Any overrides to the actual parts list data on will reflect everywhere in the drawing.

[chris]

@LT.Rusty That "works", but now you also have to "manually manage" all those BOM's where ever you put them. Wouldn't view reps or model states be an easier way to handle this?

[technologybuskirk]

Yes I would absolutely NOT want to manually update lists. I was hoping there was a way in a presentation file to assign snapshot views to individual model states in a standard assembly file. Then in the drawing I could filter the list on each page by ballooned parts and by model state or whatever. That way it would keep everything organized and always updating while only showing the parts that are highlighted on every sheet with a bubble. I cannot figure it out so far though.

[technologybuskirk]

Did you see my response to Chris?

[technologybuskirk]

I asked this yesterday but I don't think I worded it well. I'll try to state what I need and why.

1. I need an inventor drawing that shows exploded views with tweek lines.

2. Each sheet of the inventor drawing (IDW) needs to have a dynamic parts list/BOM that can automatically adjust to any changes in the assembly.

3. Ideally I would bubble the handful of things that need done on each exploded view and those bubbles would then populate the part that the arrow is pointing to updating the viewable list by sheet (using the bubble filter).

4. Every exploded view on every sheet therefore should only show what they are working with on every given sheet in the parts list/BOM.

5. On the second sheet of the drawing after the title page I only have the parts list with the item number and part number. On each sheet I would like for people to reference those numbers and lists on each sheet and have that correspond to the master list.

I have tried this by creating a presentation file (IPN), creating all of the snapshot views I want to use. I then tried to assign each snapshot view to a different presentation view in the assembly file. I might be doing that wrong, and maybe it cannot be done. But i am missing something in that process where the drawings show bubbles from every sheet and not just the sheet I am working on. Or the presentation snapshots aren't overriding every model state in the IDW.

[jeremy_wasserstrass]

The way I handle this is to make a view rep with the items I want shown in the ipn and to use in the part list on the drawing. When I make a new ipn I make sure to go to options(next to open) when selecting the assembly and select the view rep there. You can also right click on the scene and change the view rep there. This does several things for me. It allows visibility to be controlled from the assembly and makes for doing assembly steps easy by creating a new scene with a different view rep. Using the view reps like this then allows the part list(in the drawing) to be filtered by the view rep. It took way longer than it should have for me to realize that filtered part lists from the same BOM can have individual line visibility control. If you just place a generic part list on every page with no view rep filter changing a part list line visibility state affects all of the part lists.

[swalton]

I've done similar workflows and it works ok.  Revising the work instruction view reps, ipns and parts lists can be painful. 

Are you trying to have each step's part list show only the added components? 

We found it helpful to create folders in the assembly browser that contain all the components added for each step.  That made it easy to understand which sub-component was part of each step, control visibility and appearances.  We also tend to lock each step view rep. 

Once it comes time to revise the drawing, I mark up the old version to help me plan and track the changes.  I add/move the new components to the proper folders, unlock and update each design view rep and then go to the ipn.  In the ipn, I update the snapshots to show the latest view rep info. Then to the drawing.  Updating all the views is easy, but watch the parts lists.  You may have to hide unwanted row.

Please consider voting for this idea post: https://forums.autodesk.com/t5/inventor-ideas/presentation/idi-p/11701003

[LT.Rusty]

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@chris wrote:

@LT.Rusty That "works", but now you also have to "manually manage" all those BOM's where ever you put them. Wouldn't view reps or model states be an easier way to handle this?

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Unless you're replacing the models, you shouldn't have to make any manual changes down the road. IF you're just modifying the existing ones, any changes will propagate through automatically.

@jeremy_wasserstrass wrote:

 If you just place a generic part list on every page with no view rep filter changing a part list line visibility state affects all of the part lists.

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Nope- changing line visibility only affects that instance of the part list. It will not change lists on other sheets. (See, for example, the video I posted earlier- I showed the sheet 1 part list after turning off the line visibility on sheet 2.)

[jeremy_wasserstrass]

@LT.Rusty I could swear I have had issues with part list line visibility changing across sheets before. Not that it matters anymore as I have gotten more proficient with using view reps to organize how I show things on my drawings.

[johnsonshiue]

Hi! Unless there is a bug in PartsList Filter, it should just work as you wanted it. As long as the Filter is enabled, I don't see any reason why it should not work.

Please share the Inventor files in zip with me (johnson.shiue@autodesk.com) directly. I would like to understand the behavior better.

Many thanks!

[awatarius · Accepted solution]

Let me explain what I did to make this easy, and it works perfectly.

Step by step (it should be noted that you will save yourself a ton of trouble if you label everything very well).

-In my example I am using a large assembly with several sub assemblies. I am designing exploded views with a BOM/Parts list that is unique to each sheet. Everything maintains changes and is unique to each sheet. The drawing file will therefore have 14 pages starting with a TITLE Page with a base completed image, the complete BOM on sheet 2, and the first exploded view on sheet 3. These numbers and importance of these titles will be important.

1. Create/open your assembly.

2. Make any "permanent" edits or changes that need made before starting and not as you go along.

3. With your complete and updated assembly right click Model States (Primary) and select new. Rename the model State to defaultsheet1 (use your own naming convention).

4. View representations should now be propagated. Create a view representation that matches each model state. In this case the naming convention will be defaultsheet1.

5. Open the default Model State, and open the Defaultsheet1 view representation.

6. Right click the primary assembly at the top of the model browser. Click Create Presentation. This will all be defaulted to Default and Defaultsheet1 (whatever you named it). Create your snapshot in the Presentation. Save (this will be used for the title page in my drawing) and make sure the name eventually says scene1sheet1 (in my example use your own naming convention).

7. I prefer to lock the previous assembly view. In your assembly lock the previous view by right clicking defaultsheet1 and clicking lock after your presentation has a saved snapshot.

8. Right click the last used model state (in this case defaultsheet1) and click copy. This creates the next sheet with association and starts the pattern. Rename the copy to sheet2 (again whatever your naming convention is).

9. In Representations right click the last used representation and hit copy, and rename it to match.

10. Make sure both your model state and your corresponding view state are opened in the model browser. In my case I will then right click every part that shouldn't show up in the assembly 3D model (let's say everything but a frame weldment and framing hardware) and click enabled. This will disable it from this view, BOM, and so on.

11. Once everything that you don't need is disabled you then go back to your presentation and repeat step 6 naming it the next sheet to be used. In my example sheet 2 is merely an overall BOM/Parts list. So the scene will be called scene2sheet3. There is a very important difference that you will repeat for every single scene after scene 1. When you create a new scene it will ask you to select your assembly. Do so but do not hit open. Hit options. In model state (in this case it will be sheet2), under design view sheet2, and then hit ok. Now only the parts that are in those two things will show up for the scene.

12. In your presentation design your scene, capture camera, create snapshot, and save.

13. Then repeat steps 7 on.. over and over making sure to uniquely capture your naming convention and making sure when doing changes you are always in the correct model state and the correct view representation. Every time you create a new scene match the name and under options select the correct view representation and model state. Do this until you are done.

14. When you go to create your drawing you will need to place your views, name the sheets to correspond with your presentation etc. Right click each drawing sheet, and then base view select your presentation file. Make sure that the model state and view rep are also selected on each view you place. When placing your view make sure it's associative.

15. On every sheet you can then place the parts list as normal. Double click on the parts list and click the third option from the top Filters. In Define Filter Item select view representation, select the right one for your sheet (at this point the naming convention should be clear) hit the selector Limit QTY to visible components only. Hit the check box. Then under define select Ballooned items only. Hit the check mark each time and hit ok.

15. Annotate your drawing sheets as needed and balloon everything you want to show up on each sheet. 

This is the complete methodology for doing this. It's a little extra work and when typed out it looks like a lot, but it's not really that bad. Then they should update as long as you clicked associated every time you placed a view. 

[technologybuskirk]

Works like a charm