Filter User Parameters by component

[dan_brown]

Hello,

I do a lot of work with structural steel and rather than create a separate library item for each size, I store a generic shape with parameters so that I can configure as I "insert into current drawing" 

For example, I have 1 part in my library that is labeled HSS (hollow structural section steel - or square/rectangular tubing).  The parameters are for width, height, wall thickness, and length (with a calculated param for corner radius).  I insert the part into my drawing, and then set the parameters to meet the piece of steel required.

The problem I run into is when I have multiple instances.  All of the parameters have the same name, so trying identify which width, for example, goes with which piece of tubing is a pain.

2 solutions I see, which I don't believe exists, are: 1) be able to pre-pend the user parameter with a variable/property that renders out to the name of the component (for example $component_width).  2) be able to right click on the component and be able to see a table of user parameters that are only associated with that component.

I'm open to suggestions and thoughts!

Thanks,

Dan

[jhackney1972]

When inserting components which contain the same User Parameters names if you Break Link to expose the parameters you will notice the first component will have parameters with the original names.  The second component inserted in this fashion will have parameter manes with a “_1” added at the end of the parameter.  The next one will have a “_2” after the name and so on. If you remade your browser names to match you will have what you desire.

[TrippyLighting]

If you use a paid subscription, I would urge you to look at the Configurations functionality.

[dan_brown]

Thank you.  It works, but not ideal if you have several instances.  Once you rename your components, you lose the index number. You can still find it by expanding the component in the browser tree and looking at the name of the body.    Something where you can right click and see the parameters only associated with that component would be more productive.

[dan_brown]

I have a paid subscription, and have created my part file as a configuration.  I may be doing something wrong here, but it doesn't work as expected.  Let me explain.  I've created a configuration with the user parameters I need to be able to adjust the dimensions for different profiles. If I right click on my part and "Insert into current design", and then break the link so it becomes a unique component. It appears to be a configurable component, however when you look at the configuration table none of the user parameters show up.  You have to add in the user params which brings you back to the parameters table with all of the parameters showing.  If, when you clicked on the show configuration table it showed you the populated configuration table for the given component it would be great.

[jeff_strater]

If you are using configurations, you should not break the link.  That is the whole point of configurations:  To keep things associative with the original, but allow you to specify different values for parameters for different configurations.

Perhaps we are not understanding your workflow.  Maybe a more concrete example would help.

[dan_brown]

Here is my use case, maybe this will help. I’ve creates a single part that, for all practical purposes is a piece of hollow square tubing with the dimensions of 1” x 1” x1/8” wall thickness x 12” long.  All of the dimensions are stored as user parameters (Keith, width, wall_thickness, length).  A pretty simple file named HSS. 

If I need a piece of HSS (hollow structural steel) in my design I right click on the file created above and “Insert into current design”. Once it’s in the new design, I can change the value in the user parameters to change it from a 1” x 1” x 12” piece of square tubing to a 5” x 3” x 73” rectangular tubing with a 3/8” wall (just an example. ). I break the link because I do not want to affect the original HSS file. 

Using configurations and not breaking the link so everything is associated with the original model seems like a great idea within a single drawing. However, since I’m inserting the original into 100s of drawings with 1000s of sections of tubing, it is not manageable and will most likely lead to a performance nightmare. 

Does that help with a better understanding of what I’m trying to do?

[jeff_strater]

Thanks for the explanation.  I do think that configurations are meant for the use case you describe.  The problem, currently, is that you would have to create a configuration for each possible usage.  So, if  you need a 1x1x12, a 1x1x14, 2x2x12, 2x2x14 HSS, then, you would need to create a row in the config table for each of those.  Once those are set up, you just pick that configuration at the time you do Insert Component.  

There should not be a performance impact of using configurations.  In fact, it will be more efficient that using Break Link, because Break Link copies all the design data from the inserted design into the active design.  That can get very heavy.

What I suspect you really need is not there yet:  What we have called "custom configurations", and would be useful for "cut to length" type components (e.g. lumber), where it is difficult to specify up front all the lengths you will ever need.  In custom configurations, one of the inputs is "length", and rather than pick from a fixed set of lengths, you just type in a value.  Behind the scenes, it would just create another configuration, but the UI would be easier.  This is on the roadmap, but not implemented yet.

So, you have two choices:  Continue what you do today:  Insert, break link, and then it is hard to manage the parameters, or use configurations.  I don't see any other way.

[dan_brown]

Thanks for your insights. I don’t think my use case is an uncommon one and is a means of cutting the number of library items by creating a single parameterized item that can handle multiple variations  Makes for a very compact library of components vs having hundreds of variations (height and width there are multiple wall thicknesses. Toss in material steel, aluminum, stainless and you quickly have a library with 1000s of items…and that is just for hollow square/rectangular tubing. Add in round tubing and pipe, C-channel, I-beams…and you can quickly see why a single parameter driven component is desirable. )

A simple approach would be to use user parameters and be able to filter the parameters table by component name. Or when you insert a parameter driven component into the current design part of the dialog allows you to set the values. Both would be considered “nice to haves”