Single Model for Multiple Applications

Michael_Coffee

This is from an ongoing debate at work over a particular issue that I wanted to bring to everyone here and see what you think. Since there are multiple industries here, I hope someone could give some insight.

Part of our work is creating ductwork for air filtration and we will use round flanges in a few locations to bolt two pieces together. The model is, of course, very simple: it has an OD, ID, and a hole pattern. We also make the rubber gaskets for them.

Each flange may or may not be unique depending on application, but we have such a wide variety of both flanges and gaskets that use the exact same basic geometry. The debate, then, centers around: if all of them use the same geometry, why would it not be a good idea to use one model for all of them?

The main con I've heard is because of material. I do understand this from the view point that because of their application, it constitutes different models (ie. one model is a metal flange for welding while the other is a rubber gasket for securing two parts together). My contesting point is that on more than one occasion, the only difference between the models is the material.

There are two methods I've seen for entering in material. First one, you can directly assign it material from the Onshape Library. From there, this is only one choice selected and you cannot configured that material property. The second method is having a configuration table list and you choose the material from the pull-down. The table is customizable, where as the material library is not.

For what we need, we have no reason to use the material library. Baring that, I see no reason why there should be separate models. Loading times would be nearly identical, if not the same. We can customize appearance between the configurations, so that's not an issue. This model would be used in a variety of locations and would be added to as more jobs come up that require a slightly different flange and gasket. Under these circumstances, using the same model would be the way to go.

What do you guys think?

john_mcclary

By the way you can configure the material and library.

I don't recommend making a different part through configs in this case, because that would just be more hassle down the line if the following assumptions are correct:

I assume the gasket is NOT the same thickness as the metal.
I assume Only the 2D face is the same.

To me that is a new part, in this case you can just extrude the face of the flange and get your gasket with one feature.
Set it's material part number etc. and be done.

That is the typical way I handle gaskets

Michael_Coffee

@john_mcclary

Sorry, I wasn't clear when I meant you cannot configure material. You can assign material individually in the "Configured Part Properties" tab, but it cannot be used in the "Configurations" tab. Let's say you have an arbitrary number of tables of configuration options. If you assign two part numbers to the same choices from the tables, but the only difference is the material in the part properties, one of those part numbers can never be inserted into an assembly unless you insert its release, not its version.

There are a few cases where the gasket thickness is the same as a flange of the same dimensions. In my mind though, the thickness isn't an issue when it can be configured as well.

Below is an image of the model I created.

If you do not include the material table, the two models would be completely identical in principle. With the material table, everything would be condensed into one location.

Mind you, this sounds very simple in my head, but that's why I'm asking. It just seems very straight forward to me and the amount of work involved wouldn't really be any different.

NeilCooke

Here's one hokey workaround that might work:

1. Create one completely configured part and set its material manually.
2. At the end of the feature list, create a Transform/Copy in Place, times the number of material options.
3. Set each new part copy to the desired material (and change its colour and other props if required).
4. Create a Delete Part feature and select everything.
5. Configure the Delete Part feature to your material input, and edit the selections for each entry so that only 1 part ever shows.
6. When added to an assembly, if the part number field in the BOM is empty it is a new part (and you can add a PN), if a PN is present, it is an existing part.

EDIT: or you could suppress the Transform features by config rather than have an extra Delete Part feature

NeilCooke

And if you want to use "Replace" functionality in an assembly and maintain mates, you could add a mate connector before the delete part feature and configure that to each part based on material.

john_mcclary

You are right, up front there really isn't much difference in the work.
It is totally personal preference.

I just try to limit the quantity of config parameters whenever possible to avoid accidental input for the Nth instance in an assembly.