Linking best practice

[Guest rzito]

Some guidance and recommendations please.

 

I create an assembly and generate parts within it.

 

I then need to create detail drawings for each part in the assembly.

 

I drag the parts into temp catalogue then drag each part into its own new scene.

 

Then create the detail drawing for each part and one for the assembly.

 

How do I link an individual part to the assembly, so that changes to that part within the assembly update the part file and the detail drawing and additionally is it possible for the linking to be bi- directional, so the change in the individual part file updates the assembly and detail drawing?

 

Suggestions on how to manage linking to achieve a good work flow within a design would be greatly appreciated.

 

Best regards

 

 

[Guest svangeldern]

Ralph,

 

We do a Save As Part/Assembly on each part within the assembly

which creates a new scene file for the part which is then linked,

externally, to the main assembly. Our drawings for the part are

based on the individual scene file for the part.

 

This will create the bi- directional associativity that you desire.

 

Steve

 

 

[mwalls558626]

Anytime I want to work with linked files, I also do as Steve said, and save each part out from within the assembly.

 

Make sure the part in the assembly is highlighted in blue, pick "Save As Part/Assembly from the "File" menu, ( or shortcut icon ), and make sure the box is checked for it to "Link part to current scene" in the pop-up dialog box.

 

Now when you make changes to the part in the assembly, or the external part file itself, the model will update the assembly/part, depending on which file you are modifying. Make the drawing from the stand alone part, and you are set. It will update the drawing also.

 

Another option if the Scene is not too big, is to make a "configuration" view in the main scene, for each part in the assembly, and make all the drawings from the same scene using the configurations for each part/drawing. This way there are no linked files to worry about, but if the model is large, it can be pretty slow.

 

Mike

[Guest svangeldern]

Interesting....

 

I have never thought of Ralph's approach of dragging parts in and out of

a temp catalog for creating scenes for individual parts of a particular assembly

(which is why this forum is great) and being linked to the assembly scene.

 

Could this be advantageous? If so, how would you use it?

 

Thoughts?

 

Steve

 

PS Eric....Your response is mandatory.

[Cary OConnor]

Also note that you can create part drawings (I assume parts on each sheet of the drawing) without configurations or links. In the view creation dialog, select the option to pick the desired part from the browser tree. This way you can select individual parts and assemblies directly from a single scene.

 

As for the links, the comments above are correct. Also note, that you can drag a externally linked part into a catalog. That way you can reuse the same part (linked to a file) in other designs quickly (without the need to insert as link).

 

Depending on your needs, you could make due with a few links at the assembly level and use the view creation options to achieve your needs. This way it keeps the number of individual files on your system to a minimum which reduces the management aspects. If you need everything linked out, there is an option to save all part/assembly which will create a link for every part/assembly.

 

Hope that helps.

Cary

[Guest EricFoy]

... Also note, that you can drag a externally linked part into a catalog. That way you can reuse the same part (linked to a file) in other designs quickly (without the need to insert as link).

DUUUUUUUDDE !!!!!!!!!

 

he said, in utter amazement, gasping for breath, after spraying a mouthful of coffee all over his monitor.

 

Hey Cary, that was a big fat hairy ER of mine back in ought-two or three!

 

"Linked Instances in Catalogs"

 

Whoa, man... How come nobody told me about that one ?!?!?

 

Do you guys realize the ramifications, here?

______________________________________________

Now for the mandatory response:

 

I've always done the "Save as externally linked file" method. I've dabbled with configurations for part visibility in drawing views, and I still do it that way occasionally on very small projects, but if there are a number of sub-parts or subassemblies, I do the former.

 

I usually move (or save directly) the detail parts off into a subdirectory called, e.g., "PUMP9\PUMP9-DETAIL". This just helps me keep stuff straight, especially when I start getting alternate versions of parts, which I'll put into "PUMP9\PUMP9-DETAIL2," etc. Sometimes major subassemblies get their own subdirectory too.

 

Now this is important for me: Having detail parts in their own linked file gives me the added ability to put multiple detail parts on one sheet, each with its own BOM. I have a BOM template called "One-Line" that automagically brings in the part number, material, description, etc., each placed under its own respective part. This is a major deal for me.

 

I kinda have a hard time with configurations. When assemblies get involved, the configurations of the sub-files, how they're inherited and treated, etc., etc., starts to really hurt my little head. A couple times I've found myself in some kind of configurational iterative non-reentrant counter-recursive loop situation that gets me reaching for the Prozac. So I keep it simple, and don't use configurations very much.

 

[tlehnhaeuser]

One more note - There is now the option to save ALL parts as external links from a top assembly. This saves having to select each part and save out.

[scoelho]

ok, so we do the same thing here. one assembly scene with all the parts, then "save as external" each model with a link. Then detail each part from the single part scenes.

 

In the assembly scene, you can expand a part or go to part properties and see where the individual part is linked to..it gives you the directory path info. So from the assembly scene you can find all the "linked out" files and their locations.

 

However, if you open the individual part scene, there is no way (that I know of) to find out if the part is linked to a assembly scene somewhere. This has caused some minor problems for us in the past. Someone opens up a individual part scene, makes a change, and unknowingly alters a assembly scene somewhere.

 

any thoughts on this?

 

-Steve

[tlehnhaeuser]

In the assembly scene, you can expand a part or go to part properties and see where the individual part is linked to..it gives you the directory path info. So from the assembly scene you can find all the "linked out" files and their locations. IRONPRO OFFERS THE EXTERNAL LINK MANAGER THAT WILL PROVIDE A LIST OF ALL EXTERNAL LINKED FILES IN A SCENE.

 

However, if you open the individual part scene, there is no way (that I know of) to find out if the part is linked to a assembly scene somewhere. This has caused some minor problems for us in the past. Someone opens up a individual part scene, makes a change, and unknowingly alters a assembly scene somewhere.

I THOUGHT IRONPRO WILL DO THIS BUT APPARENTLY IS DOESN'T UNLESS I UNCOVERED A BUG.

ALTERNATELY IS YOU IMPLEMENT DESIGNDATAMANAGER YOU CAN ACHIEVE THIS, HOWEVER YOU WILL NEED TIO OPERATE IRONCAD WITHIN A DATA MANAGEMENT APPLICATION. THIS MAY OR MAY NOT WORK FOR YOU DEPENDING ON YOUR DESIGN ENVIRONMENT. IF YOU WANT TO TRY, YOU CAN DOWNLOAD A FREE LICENSE OF DDM FROM THEIR WEBSITE.

 

 

any thoughts on this?

 

-Steve

27612[/snapback]

 

[tlehnhaeuser]

As for the links, the comments above are correct. Also note, that you can drag a externally linked part into a catalog. That way you can reuse the same part (linked to a file) in other designs quickly (without the need to insert as link).

27605[/snapback]

 

Cary, this is great and even tells you that its linked. Now, is there a way to drag the file to catalog WITHOUT being linked with a hotkey?

 

Otherwise, I need to Edit Catalog PArt > Unlink> Save > Rename. Not a major issue, just thought its always good to ask for hotkeys.

 

[Cary OConnor]

Actually it looks like there is a regressing in XG. It use to ask the user to maintain or break the link when you drop a linked part into a catalog. I will file that so that it works again to give this option.

 

Cary

[mwalls558626]

Yes, Thanks Cary. It is important to have it ask for the maintain or break link. Real important......

 

Mike

[Guest rzito]

Thank you very much to all the respondants

 

You've given me some great guidlines, which should increase my productivity and streamline my work flow.

 

Best regards

[Guest svangeldern]

Also note that you can create part drawings (I assume parts on each sheet of the drawing) without configurations or links. In the view creation dialog, select the option to pick the desired part from the browser tree. This way you can select individual parts and assemblies directly from a single scene.

27605[/snapback]

 

Cary,

 

When I create a detail drawing as you describe above the icd is over 10,400 KB (the assembly ics is 14,500 KB and the icd of the entire assembly is 13,159 KB).

 

If I save the part externally and recreate the drawing linked to this individual part the icd file size 327 KB (ics is 89 KB).

 

I like the ability to select an individual part from an assembly for detailing however

if each icd is going to be the size of the assembly I don't think it is worth it.

 

Are these large icd file sizes to be expected if this method is used?

 

Also....If I create a drawing as before and CTRL-SHIFT-L to change the link from the assembly.ics to the individual part.ics, IC fails to generate geometry for any of the views.

 

Thanks,

 

Steve

XG64, W7

[Cary OConnor]

Using the single file approach to creating drawings will produce a larger drawing since it needs to store the scene file data with the drawing.

 

The external linked files will have smaller drawings that reflect the size of the scene file.

 

I guess the question is how will it affect you if the file is large? Are you sending that ICD around or just a finished file? Also, can you create mulitple sheets in a single IDC for the parts instead of multiple individual drawings that are large in size?

 

The Ctrl-Shift-L issue makes sense. You are creating a view from the overall assembly of a part within. If you switch to the individual part ics, the view will not understand that part (since it is just the part and not the assembly/part path to the geometry).

 

Cary

[Guest svangeldern]

Cary,

 

Thanks. Makes sense to me now.

 

Steve