Hello
Under SW, to make 1 finished part from a blank, I chose the "Insert part" function in a part file, then carried out the machining by functions.
I find 2 main disadvantages:
1) In the design phase, replacing the stock with another destroys a lot of the link with the machining functions.
2) In the PDM explorer, the architecture is not displayed in the "Used in", "Content", and "BOM" tabs.
So I'm thinking of doing it in assembly. If anyone has ever done it??
Slts
YP
Hello
I think you have to use the configurations: you can use the same part and change the configuration in the assembly:
https://www.youtube.com/watch?v=7zv6OxE0qyw
Instead, we use the derived configurations for crudes:
http://help.solidworks.com/2013/French/SolidWorks/sldworks/c_Derived_Configurations.htm
Otherwise, the configuration help page:
http://help.solidworks.com/2014/french/SolidWorks/sldworks/r_ConfigurationManager_configurations.htm
Hello
Without EPDM, I inserted a part into a part ("by hand" nomenclatures).
Since I use EPDM, I insert the part into an assembly, which I dimension and use as a part. It effectively allows you to know the use cases, and simplifies the changes of the basic gross. On the other hand, if you replace your stock with an element that is not from the same database (file copy, therefore same internal ID), you will also have problems with lost references.
It works well for machined parts, but if you want to use blanks to make welded constructions, it complicates things, because suddenly you have to make your design at the level of an assembly, so without the "welded constructions" functionalities available at the level of a part.
@.PL, in general with EPDM, you avoid managing configurations on this kind of thing.
If you have an article code for your stock and article codes for your machined versions, if you managed it at the level of a single part via configurations, it would imply that you would pass a hint on all your articles when you only evolve one! Or you don't use the indices feature by EPDM and you manage it the old way, but you do without one of the arguments of the system, plus all the limits that this implies on the workflows !
Hello
We use this method.
There are workarounds for the 2 disadvantages:
For the 1 it is enough to never link the machining to the references taken on the stock but use a pilot sketch + pilot plans to do all your material removals. This way, the machining is completely independent of the workpiece. It's heavier to do at the beginning but allows you to change the stock along the way without losing your functions (they just get wrong if they don't cross the model anymore)
For the 2 you just have to use the 'used in' tab but the report generator tool with a .crp report that looks for dependencies. We had to make one in order to be able to find the use cases of parts used in virtual sub-assemblies (functional sub-assemblies that are used to model the different positions but which do not have a drawing and therefore that are created virtually to simplify copy operations)
Example of our generator for the use of a file called R26165*:
In yellow, files using it (the machined part in this case). The result of the generator can be exported to excel to do more advanced sorting if necessary (if there are a lot of use cases).
Machining in an assembly is much more limited (although SW has added a lot of functions in recent years)