I'm having a problem creating my part family on SolidWorks 2019. I can indeed make my configurations, and create my family of parts automatically, but I can't manually enter the sketches using D1@Esquisse1 (for example).
Quite normal until then, since I have to specify the name of the component after the sketch; so I tried D1@Esquisse1@OUTIL^POSALUX-CONCAVE<1> but nothing helped.
The only solution so far is to create a constrained sketch in the assembly, and use it to get the dimensions. Isn't there a cleaner way to do it? Because the command $CONFIGURATION only gives me the name of the configurations.
A picture that speaks better for itself, where you can see the "TOOL" part with the extrusion, and the "PART FAMILY" sketch, completely constrained by the extrusion sketch, bringing the dimensions of the drawing into my part family.
as @Julien MARTIN says, it is normal that you cannot edit the dimensions driven by the part family in the sketch, this is a default setting of SW to avoid modifying the part family by accident, to allow the modification, you have to "right click" on your part family, "Edit Function" and change the "Edit Control" setting. The external reference we can be an influence too!
I can edit my sketch dimensions by right-clicking, then "Edit function", or I enter all my values at once. On the other hand, these values are not displayed in my part family (even in automatic creation), hence the creation of a sketch in the assembly in order to use values already existing in my part.
I can't enter my values on "Sketch1" of my "Boss.-Extru.1" function of my part [Tool^Posalux...] in the part family. I am forced to use the annex sketch "PART FAMILY" (on the photo of the first post).
If you already have different lengths of this dimension in a family of parts, you should not control its length from the assembly but control the configuration of the part with the right length.
I'm not sure I understood your answer, can you comment on my family of parts in the attached photo? The D1-D4@FAMILLEDEPIECE correspond to my sketch in the assembly and the values I would like to display without this sketch.
First, try to put the machining functions (fillet, chamfer, drilling, etc.) in the parts and not in the assembly as you did. If the geometry of the parts changes, it will prevent you from having the assembly functions in error.
Second, make your life easier. Since you have created the configurations in the "TOOL" part, there is no need to create an additional sketch in your assembly. All you have to do is call up the configuration in your part family and delete the columns that drive your "PART FAMILY" sketch (see my example).
Keep in mind that your design will evolve over time, and the more you complicate your assembly, the harder it will be for SOLIDWORKS to calculate. Here you only have 3 simple components but imagine if you have thousands! In addition, it will be easier for you to find your way around.
Anyway, that's my vision of things, it's up to you.
