Hello
Inventor allows you to link your models to an external XL file.
Advantage, you can manage a lot of things (you have all the functions of XL), you are sure that the same formula/values are used everywhere, it's practical: you duplicate the folder, you modify the values of the XL file (no need to know Inventor) and the model is updated.
Do you know if a similar possibility exists with SW?
There is indeed Driveworks but it seems heavier to me to set up? not to mention it's an extra cost.
You can go through a family of parts, which controls either the length of several parts or assemblies (with possible formulas) or a skeleton in the form of a sketch that will drive your parts or assemblies.
Edit: with the Mycadservices tools you also have access to PilotAssembly:
https://help.visiativ.com/solidwatch/2022/fr/PilotAssembly.html
The part family is not suitable: too small, unless I have missed something. In addition, the goal is not to manage configs...
In the case I see, the XL file controls both the parts and the asm, whether it is the dimensions or the presence/absence of parts.
PilotAssembly seems to do the job but much, much less flexible.
To detail how you work in Inventor:
- the XL file is associated with the prt/asm file;
- In the prt/asm file, on the Equation page, the variables defined in the XL file appear automatically.
- it is easy to associate the desired variable of the XL file to a dimension (we type =, we type/choose the name of the variable from a drop-down list).
the only constraint is to respect a particular layout for the XL file: the variables are in a column, the system stops browsing the list when it encounters an empty cell. For the rest, we do what we want around us.
You can also go through equations linked to an external file, but it's a text file so it's less flexible than Excel.
For the part family, you don't need to have several configurations for it to work. (even if it's indeed a roundabout way of using it)
I've already used it in this sense and you can control from one assembly several parts and assemblies quite easily while adding formulas between different dimensions.
On the other hand, the columns with formulas must be located after the columns that drive a coast, otherwise it will cause a stir.
I agree with @sbadenis on PilotAssembly. It's the tool that can match all your requests. But yes it is less flexible to use according to what you say about the Inventor tool, and it will require you a lot of work on the 3D.
Hello
I have been modeling homothetic molding tools for a very long time using an external excel file to which different parts of an assembly are linked. It works very well. Here's how to do it:
Create a part family file with the sketch dimensions that need to be controlled. To be more comfortable, copy all the cells into a blank excel file and work outside SW.
Create another excel file, save this file in a special and dedicated rep.
You'll enter the dimensions of all your parts into this file.
Tile the two files so that you can switch between them.
With the part family file, in the value cells, switch to formula mode (=) and point to the cell in the input file. A link is created between the two cells of the 2 files. Do this with all the dimensions.
Copy all cells from the external part family file into the encapsulated part file.
To reconstruct the parts, it will be sufficient to edit the families of parts and to have the input file open. All linked values will update. The only downside, which I haven't found a solution to, is that the input file must have a fixed path otherwise the links get lost. At the end, you just have to make a copy in the 3D directory to be able to reuse it by overwriting the reference file.
Everything can be controlled, the fcts, the rehearsals, we can set conditions, operations...
I hope I have met your need.
@phamnuwen: Very interesting.
As soon as the opportunity arises, I'll try it. I will have to dig deeper into the question of paths, for the client I am thinking of it must be simple to manage.