Modifying a Part Reference Inserted in a Part File

3D Design Volume Model
1

Hello

 

A problem arises for me.

Within my company (an aluminium joinery design company) we model according to a rather particular method.

We model what we call nodes, which are the assembly of two profiles. We insert these different nodes into a part file using the insert => part command. Following the insertion of these knots, we link them with an extrusion in order to reconstitute our bars constituting our joinery. See sample file attached

However, if I replace one of the nodes, I can't change the reference in the part file. In the attached example, let's say I want to replace the angle A with the angle D.

 

Do you have a solution for this ??

 

I got my way through EPDM, but the downside is that if I have multiple identical nodes in the same file, I replace all the nodes but I can't modify just one node.

 

Thank you in advance for your contribution

 

 

Kind regards.


test_modelisation_par_noeuds.zip
2

To change the reference of these inserted parts, you must first of all... close the room...

 

Then, via the "open" window, point to the room where you want to change its references and click on the "Reference" button (see attached image). You can then redirect the references (Double click on the name of the part or on its path).

 

You validate and open the room in the process.

 

That's it.

 

If you work with EPDM, you must of course extract the part beforehand.


screenshot067.jpg
5 Likes
3

Hello

Why not use assemblies?

I only see advantages: modularity, nomenclature, drawing, modifications...

 

But I guess I don't have all the keys.

 

1 Like
4

@Benoit.if

 

Unfortunately this way does not allow me to modify a single reference when a reference appears several times in the same room. Because when a reference appears several times, it groups it into a single line.

 

See attached screenshot.

 

@rmorel

 

This modeling strategy was put in place because at the level of the design office a complete joinery is considered and not a set of assembled bars making up the joinery.

In addition, our joinery being configured according to a family of parts, we use a macro to separate the different configs in different part files, macro not working with assemblies.

Another important fact, I am almost the only non-novice SW user, so each manipulation must be quite simple to implement.

 

However, if anyone has a modeling method to propose, I'm all for it.

 

 


sans_titre.png
5

Hello

 

Manually to replace only a component used several times in an assembly but you have to open the document, You have to use the "Right click/replace component" option

 

Otherwise with the APIs it is possible to make the modification with the document closed.

You must use the swDocumentMgr library with the API: Replace Method (ISwDMComponent6) 

Or with the document opened with the API  "ReplaceComponents Method (IAssemblyDoc)"

 

examples are available in the API help

 

Philippe

3 Likes
6

Ah OK, we didn't see that with the example.

 

So, it seems compromised...

 

One method that could be used would be welded construction. This would also make it possible to have a nomenclature of flows.

7

Why not have created "templates" (a standard base) of complete joinery in assembly: each element being a part file.
In addition, you can add hardware (in particular to generate a bill of materials as @rmorel)

 

Once the standard database has been made, for each new customer, make a take-home composition or from the EPDM make a copy of the tree structure (in tools), rename all the parts files and the drawings.

Then dimensionally modify the client assembly.

8

Using the library function in Solidworks (welded construction)

 

See attached link

http://www.lynkoa.com/tutos/3d/fonction-bibliotheque-dans-solidworks

 

This allows you to create an auto cut via the profile you want, it's up to you to set it up

if parts # ref #

 

@+ ;-)

9

@Benoit.if

It's a mix of the two, we use the welded mechanic to create the knots. Mia s simple extrusion to bond knots.

 

@flegendre

The design of standard elements is on the shelves but it will take time for us to put together something effective. That's why I'm looking for a palliative solution.

 

@gt22 I look at your link as soon as I have some time...

 

Otherwise, there is no solution to replace a single occurrence of a reference???

 

 

 

10

If, for example, you create only one ANGLE file.

In this file you create a series of configurations (ANGLE A,B,C,D,.......)

You insert the Angle piece into your frame (which you place in your 4 corners).

Then you play on the config of the ANGLE room independently in your 4 corners.

 

To do this: right click on the ANGLE part

Have External References List

then change the config


ossature_test.png
2 Likes
11

@gt22.

 

I just looked at the link on library functions.

I tried to use this way of modelling, the only problem is that our profiles are complex profiles (compared to an IPE or other structural profiles) and the cuts used are only slightly standardised and standardizable.

 

The complexity of the profiles makes the implementation cumbersome and complex, and requires manual rework for the rest of the operations (drilling, and other profile routing elements).

12

no matter how difficult it is via intelligent component you must be able to make the reservations that must be made to the nodes

at least that's what I think

you don't always have the 2 profiles with cutouts and even if it was the case

A line of Jupiter can do it very well in car I think 

@+ ;-)

13

@flegendre.

 

Indeed, this technique can be suitable for some of my cases. Unfortunately not the entirety.

For the rest of the cases, I'm afraid that there is no real solution (except to see the creation of a macro capable of entering the link paths and modifying it.

 

I will test this method so that I can then deploy it in my company. But indeed it seems to me more than vialbe.

 

Thank you for your help.

 

Happydad