MULTIPLE PARTS ON A SINGLE DWG

[davesonger]

I am trying to do the multiple part insertion on a single page with all parts showing up on a single BOM. I am having trouble getting them to come in to the dwg seperate instead they all come in as a group. I have set up LOD for each part but still they come in as a group. Its very frustrating, can you please take a look at my attachement and see what you think it could be that I am doing wrong. The files are from IV 2011.

Thanks Group

David

[alessandro.gasso]

Dear David,

I’m not sure I’ve understood your request.

By the way, I hope the video attached could help to get what you need.

If not, please, provide more details about the result you would like to achieve.

Many thanks.

Kind regards.

Alessandro

[davesonger]

Alessandro,

Glad to hear from Autodesk on this. I am still having problems getting it to work on my end. Your video is exactly what I am trying to do. If you could provide a small text based instruction that would be GREAT as the video moves kind of quick. I am also having trouble with those parts as far as the centerlines showing up in the dwg and when a projected view is done the holes do hot show up as dashed lines in the projected view?

Thanks Very Much Alessandro, for your assistance here, as this is a core Inventor Task that I will use all of the time.

Also one question, is there any drawbacks to making all of the components in the assembly a Weldment and then placing the individiual components into the dwg under the Model State Tab, then under Preparations sub tab?

Thanks So Very Much For you Help

David

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[alessandro.gasso · Accepted solution]

Dear David,

Please, find below the steps I show in the video.

• In the assembly file

1.  Activate the LOD 12x12 BASE PLATE

2. Select the components END CAP BACK and END CAP FRONT, right-click, Suppress.

3. Save the assembly.

4. Repeat steps 1, 2 and 3 for the LODs END CAP BACK and END CAP FRONT, of course, selecting and suppressing the components you don’t want to see in the LOD.

• In the Drawing

5. Base view.

6. In the Drawing View dialog, Component tab, select 12x12 BASE PLATE in the Level of Detail field.

7. Repeat steps 5 and 6 for the Level of Detail END CAP BACK and END CAP FRONT.

Now you have three assembly views, each one displaying just on component.

8. Annotate tab > Parts List.

9. Select one of the views.

10. In the Parts List dialog select Parts Only from the BOM View drop-down menu, OK and place the Parts List.

Please, let me know if you need more details about the video.

About the other two problems, I’m sorry, but I’m not sure I’ve understood them.

Please, provide me more details about them (i.e.: some example files) and I’ll be happy to assist you further.

Many thanks.

Kind regards.

Alessandro

[davesonger]

Alessandro,

Thanks for your response....I have it now. The only reason that I was doing the Multiple Parts like this on a single page and adding them into an assembly was to get the BOM to have all of the parts on it in one BOM.

My original dilema was, I was just inserting IPT files into a dwg sheet which is very simple. But when you make the BOM you are stuck with making a BOM for each part. Is there another way to accomplish this single BOM issue on a sheet with Multiple Parts, rather than going the LOD Method. It seems more natural to be able to just drop IPT files into a sheet and get one single BOM for all items on the sheet? Now bear in mind, these parts would not be related to each other, but would be in the same project file. It seems to me the BOM is the weak link here, unless I don't see something else.

Thanks Very Much for your help.

David

[swalton]

The container that holds multiple parts is an iam not an idw.  There is no easy way to add the parts to an idw and get a BOM.  How would you show that you needed 12 of part A and 2 of part B?  Place 12 views?  In the iam file, just pattern part A 12 times and hide all but one with a design view.

I would use a design view rather than a LOD to show the individual parts in the assembly.  Having the iam and multiple views at different LODs has caused issues with saving for me in the past.

[alessandro.gasso]

Dear David,

When you talk about BOM you are talking about Assemblies.

By the way, for accomplish what you need, the LOD are not necessary.

You can do the following.

1. Create a new drawing and create the views of different ipt files.
2. Open a new dummy assembly.
3. Place Component
4. In the Place component dialog, set Autodesk Inventor Parts (*.ipt) in the Files of type field.
5. Then, windows select all the ipt files and click on Open.
6. Save the assembly.
7. Switch back to the drawing create in step 1
8. Annotate tab > Parts List.
9. In the Parts List dialog click on Browse for file and select the assembly file created with steps from 2 to 6.
10. In the Parts List dialog select Parts Only from the BOM View drop-down menu, OK and place the Parts List.

I hope you can find this useful.

Please, let me know if you need more details about the procedure.

Thanks and regards.

Alessandro

[davesonger]

Allesandro,

This procedure seems faster than the LOD method, I will give it a try and let you know how it works.

Thanks Very Much for your response.

David

[davesonger]

Allesandro,

Will this method work if you have to attach Part Ballons to the different parts on the sheet? what I mean will all of the part balloon numbers match the BOM(Parts List)?

Thanks

David

[alessandro.gasso]

Dear David,

The balloons numbers will match with the ones of Parts Only BOM from the assembly created with steps from 2 to 6 of the last procedure suggested.

Please, let me know if this doesn’t answer to your question.

Many thanks.

Kind regards.

Alessandro

[alessandro.gasso]

Dear David,

Reading more carefully you last question, I think I have to clarify some points.

If you apply the balloons to the views of the parts in the drawing created in step 1, all the balloons numbers will display as 1, because they take the value from the ipt file.

So, what you can do is to select all the balloons, right-click, Edit Balloon, and override the numbers in the way that match the items numbers of the Parts List inserted in steps 8 and 9.

Another limitation here is that you cannot use the Auto Balloon.

One tip, if you decide to use this method anyway, is that, if you need to select a large number of balloons for overriding the numbers, you can window select them setting a custom filter for the selection with the setting you can see in the attached images.

Please, let me know if I can help you further on this.

Thanks and regards.

Alessandro

[davesonger]

Alessandro,

I had thought that this was going to be the case, of editing the Part Balloons as they would all read the same number. There basically will not be any intelligence between the Balloon and the Part with this method of part assembly. Moreover, if a part is changed then updated on the sheet, its balloon number would probably reset back to 1? This would/could cause for alot of manual monitoring and editing.

Thanks Alessandro, I believe the LOD Method, however longer, is probably the best way to go as the part intelligence is still in tact, even through part edits.

Thank You Sir for your effort on this

David