Small problem that poisons my life: in the context of a mechanically welded part , when I insert a part (screws) with several configurations (a part in a part: yes doable...), I can't find the right reference in the list of welded parts of my drawing. Impossible to modify it directly in the properties of my welded parts list, the field remaining empty even if I enter the text manually... I also tried to modify the properties of my screw but nothing helps.
Hello, if I understood correctly the solution is: In the inserted part (screw in your example), you have to "list the external references" to have access to the configurations.
SELECT A CONFIGURATION IN INSERT PART MODE ON SOLIDWORKS
Is there a way to select a configuration in Part Insert mode on SolidWorks ?
Another topic from the Lynkoa forum . We found this question interesting and many SolidWorks users may not be aware of this possibility.
Indeed, when you insert a component into a SolidWorks assembly, it is possible to choose the configuration in which you want to use the component. But when you are in the part mode and want to import a 3D component, is it possible to choose which configuration to use?
Let's take the example of this fastener which contains 3 configurations:
When a symmetrical part is created from this component (function: " Insert ", " Symmetrical Part ") the resulting part will automatically inherit the configurations of the initial component (provided that the link with the source is not broken).
Similarly, when working in the " Part " context, it is possible to insert 3D components ("Insert ", " Part " function ). Once the component is inserted, to select another configuration, simply right-click on the function in the creation tree and, from the drop-down menu, select " List external references..." and choose the configuration to use (provided you do not break the link with the source).
On the initial part, if changes are made in the configurations (removal of certain configurations, addition of configurations):
Regarding the symmetrical part generated from the initial component, the inherited configurations are not modified (adding, deleting), the configurations are created at the time of the creation of the " Symmetric Part" function. However, it is still possible to right-click on the function in the design tree and select another configuration via the " List external references" dialog box. Deleted configurations remain active in the symmetrical part, but are no longer visible in the list of external references.
For the derived part or the part inserted into a 3D component, the configurations have not been created automatically and therefore the list in the " List External References" dialog box remains up to date.
With the 2012 version, if you want to display a "part number" property in a part list, the "Customize" property and not "Configuration specific" is taken into account.
If you want to "list external references" the inserted part must be open.
The problem is not to choose the right config but that the properties of the body appear in the table obtained by right-clicking/property on a body in the list of welded parts.
I just tested, we get this: a property with a value of "fromparent+"
knowing that in my part file, I created a personal prop "DESCRIPTION"
I was asking for the choice of the config to be sure that we are talking about the same thing.
Once again, which version of SLD?
I've already had this pb, answer from Axemble: bug of the 2012 sp4 version you have to switch to sp5 or 2013
In your Stefbeno case, solidworks uses the DESCRIPTION property of the Customize tab, so if you have a different description for each config (Custom Properties tab), solidworks doesn't take it into account.
For the +fromparent problem, you should not check Custom Properties, here is the Axemble solution for this:
To retrieve the properties, the parts must be in context. the parts that are inserted and that are in the context , applies its properties to the base part, Only if the property name is not already present in the Part Properties.
In your case there is a problem
To resolve the issue, you need to update your SolidWorks 2012 SP 4.0 to SolidWorks 2012 Sp5.0 or 2013
Be careful checking the Custom properties can create problems! (see previous message)
I don't know why solidworks doesn't use configuration-specific properties but it's a big problem especially with welded constructions because you can't use configurations with different designations.
You have to use the Customize tab, which in my case is annoying because with EPDM you find yourself having to fill in the 2 property tabs while there is an option to disable the custom properties page (@)
A priori, therefore, I can't do much with this +fromparent. I've always had this problem, despite all the versions of SOLIDWORKS I've used. For your information, I'm using the 2013 version.
I'll try by creating a simple file for each type of screw. We'll see.
I'm still leaving the post open in case I still have people with good ideas.
I partially solved my problem even if the solution doesn't suit me but hey...
I deleted the configuration table, then each configuration of my screw file, keeping only the one that interested me. In the personal properties of my remaining config I deleted all the variables in the general tab and in the config specific tab.
This allowed me to MANUALLY enter the "description" value of the body in my list of welded parts of my mechanically welded part file when before I couldn't!
Not very conventional but, a priori, effective.
On the other side of the coin: I have to create a screw file for each type inserted...
