Material management in a component family

3D Design Volume Model
1

Hello

I have created a family of parts via an Excel file by associating custom properties. It works up to the following limit:

- one of my custom properties corresponds to the nature of the material ($PROPRIETE@MATERIAU) that I have entered for all the configurations in my file (example: AISI 304).

When I view the properties of a configuration (File, Properties), in the "Configuration Specific" tab, I see the name of the property "MATERIAL" and its associated value "AISI 304".

I would have liked this information from my Excel file to be able to modify the "material" field of the Feature Manager but it doesn't!

When I right-click on this "material" field to configure the material, I open a "Modify configurations" table which offers me:

- a "Material" column, equipped with a drop-down list in each configuration field

- my column previously created in Excel "MATERIAL"

This "Material" column equipped with a drop-down list requires you to check each cell to inform the chosen material. My file includes 300 configurations (so 300 lines to fill in), it remains a heavy update operation to perform while my Excel file produces similar information.

 

Questions:

Is there a way to retrieve the MATERIAL info of the part family to update the material of each part configuration?

I don't understand how to handle the links between the configuration change tables and the Excel files of custom properties.

Can you enlighten me?

Thanks in advance,

 


extrait_mofif_config_sw.jpg
1 Like
2

The best I think is to create you

_1 part family per material

in a personal library folder  

x sub-folder materials

or configuration of materials in a family of parts see this link

http://help.solidworks.com/2013/French/WhatsNew/wn2013_Configuring_Materials_in_a_Design_Table.htm

@+ ;-)

 

1 Like
3
Hello, yes it's possible, you have to use the column header "$LIBRARY:MATERIAL@part_name" more information:

In SolidWorks 2013 onward, using the new design table functionality, materials can be assigned to single and multi body parts per configuration.

The column header uses this syntax:

For a part: $LIBRARY:MATERIAL@part_name

For a body in a multibody part: $LIBRARY:MATERIAL@body_name@part_name

Spring:

http://help.solidworks.com/2013/English/WhatsNew/wn2013_Configuring_Materials_in_a_Design_Table.htm

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4
Spring:

http://help.solidworks.com/2013/English/WhatsNew/wn2013_Configuring_Materials_in_a_Design_Table.htm

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5

Hello again everyone,

With a little goodwill and with the leads you gave me, I even managed to get to the end of the subject.

In my excel file, I added a column named "$BIBLIOTHEQUE:MATERIAUX@le_nom de_pièce".

For each configuration (line), I filled the cell with "solidworks materials:AISI 304".

I made the links that go well between the "piece.sldprt" and the excel file and the result is as follows:

AISI 304 does appear in the material field of the feature manager.

PB solved!

Do you think it would be worth a tutorial?

Slts to all.

6

Hello

A tutorial why not but what would have been good is to put @PL in good answer he is the one who gave the solution, it would have been cool to reward him.

@+

 

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7

@ coyote yes I agree with you

The link posted seemed clear to me too

That's how it is

@+ ;-))

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