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Open all parts in assembly at once

10 REPLIES 10
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Message 1 of 11
Paul-tedecon
4170 Views, 10 Replies

Open all parts in assembly at once

Hello all,

 

is it possible to open all parts in an assembly at once?

 

I tried to select them all in the modelbrowser, and then open, but ain't working. I tried also with the design assistent, but also not working.

 

I will use this function to place all (open) parts from an assembly in one drawing. Then i am sure that i don't forget any parts.

 

Or is there maybe another solution for my problem?

 

Thanks in advance,

Paul van Deursen

10 REPLIES 10
Message 2 of 11
Cadmanto
in reply to: Paul-tedecon

Paul,

How many parts are we talking?

What is your final drawing wanting to look like?

 

This might be a candidate for an ilogic rule.

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


Message 3 of 11
Paul-tedecon
in reply to: Cadmanto

 

Thanks for your reply.

 

 

 

We’re talking from 10 to around 90 parts and all assemblies are different (totally different).

 

 

 

I want a front and maybe sideview from each part on one drawing. For this customer we need to export all parts to autocad, place them on one sheet and dimension all parts following their dimension style.

 

 

 

A tool to automatically open all parts, will already safe a lot of time, then I only have to place them in a drawing.

 

 

 

Hope this gives an answer on your question?

 

 

 

This is actually the first time I hear something about ilogic rules. What will it do?

 

 

 

Thanks!

 

Message 4 of 11
JDMather
in reply to: Paul-tedecon


@Paul-tedecon wrote:

 

I will use this function to place all (open) parts from an assembly in one drawing. Then i am sure that i don't forget any


Just to clarify - this is all parts on one drawing sheet in one dwg file?

Not multiple sheets (one per part) in one dwg file.
Not multiple dwg files (one per part).


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Message 5 of 11
Paul-tedecon
in reply to: JDMather

Indeed, all parts of one assembly on one sheet exported to dwg.

 

Unless there is not enough space on a sheet, but then i will make another dwg with the rest of the parts on it.

 

Thanks!

Message 6 of 11
R.Corriveau
in reply to: Paul-tedecon

You can open multiple parts from explorer but not the assembly browser.

 

IMO: That many parts detailed on one sheet is a bad practice.

 

 

Message 7 of 11
harco
in reply to: Paul-tedecon

You can export the bom to excel and use as a checklist.

You could also pack and go the assembly to another folder to gather all parts in one place.

You could add a custom iproperty to all the parts and show in the BOM editor, when the part is included in the drawing fill in the iproperty with yes,done, drawn...etc. as an alternative checklist.

 

One thing I wouldn't do is open 90 individual parts at once, my machine would choke after about 30.

Yours may be a super duper machine.

I normally only open about 10-20 if it's necessary to do common action on them all.

 

I know the customer is always right even when they are wrong, we have them asking for all parts on one drawing too, but I agree with the other lads, too many parts on one drawing is asking for trouble.

 

A final option would be view reps in the assembly to isolate the parts in the drawing, but this is time consuming.

Message 8 of 11

Hi Paul-tedecon,

 

As others have mentioned, the practice of placing all of your model drawings into a single drawing file is often poor practice. But here is a simple ilogic rule to open all of the referenced files from the assembly.

 

'Define the open document
Dim oDoc As Document
oDoc = ThisDoc.Document
'Look at all of the files referenced in the open document
Dim docFile As Document
For Each docFile In oDoc.AllReferencedDocuments                
'open the indexed file
'true opens the file normaly
'false opens the file programatically without generating the graphics
ThisApplication.Documents.Open(docFile.FullFileName, True) 
Next

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

Message 9 of 11

Is it also possible to open all parts include drawings in an assembly?

Message 10 of 11

Awesome code, does exactly what I need it to do. Thank you so much!

 

I'm going to piggyback off of this solution if someone else can lend a hand with code or methodology (I'm just getting into the guts of iLogic, still a beginner)

 

As part of our sheet metal workflow, we need to open parts, run an iProperties macro to update the sheet extents (length, width, height, etc.), save the part, then close it.

 

For example, if I have a pice of 1/4 x 1/4 x 4" bar stock in an assembly i just updated to 5" long. I'd have to go into the part, update the part description using a hotkey, save the part, and close it again. We have to do this with EVERY sheet metal part in an assembly and it tends to be a lot of clicking and wasted time.

 

I really want to use this code to open every part, update every part description (go to sheet metal flat pattern, run the update description hotkey, press enter, save), and then close it again. Any ideas on how to get there?

 

I'll keep tinkering away at this as I go, but any advice is appreciated. Thank you!

 

-Steven C.

Message 11 of 11
ThomasB44
in reply to: lazerboy

Hi @lazerboy

You could create an iLogic rule to update your description field in iProperty like your macro do it.

This rule could be set with an event trigger on "before save".

And you could do this in your sheet metal part template.

 

With this workflow, each of your sheet metal parts will be updated automatically, and no need to open and close some parts, just save, and the rule will do the job.

To set the event trigger to all your old parts you can use code injector :

http://beinginventive.typepad.com/being-inventive/2012/02/injecting-ilogic-code-and-ilogic-event-tri...

 

Say me if you need help to create the rule.


Thomas
Mechanical Designer / Inventor Professionnal 2023
Inventor Professional EESignature

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