Adding custom property to design table

[tmox]

I created an excel spreadsheet with all configuration information. Created the default part in SW and then created the design table "from file". I further want to use the property manager to filter the configuration list so that i can use this part in my library. the configurations come into the file fine and work well.
I want to use DIAMETER and LENGTH as the 2 custom properties and put them in the form $prp@DIAMETER in my spreadsheet. When i use the property manager it fails to recognize these columns as selectable properties. Can someone say what i am doing wrong.
By the way none of the properties i want to filter by are dimensions in my model.

 

[drawoh]

tmox,

If you have an empty columm to the left of your custom property columns, SolidWorks will not read them.

It is not obvious to me what you are trying to do. Are you trying to add DIAMETER and LENGTH as custom properties, or as configurations?

JHG

 

[tmox]

JHG,

Ultimately i want to put this part in the library. The file will contain a hundred configurations.
I want to use the property manager to filter the configurations and i want to select length and diameter as my filters. Neither of these parameters is a dimension in my model but, are relevant on the spreadsheet.
When i use propery manager, it fails to recognize these parameters and doesn't allow me to select them as filters. I don't know why.

 

[ArtemTat]

Do you have this fail while creating Design Table? Or they are invisible while creating Property Manager Page?

Make sure these parameters can be controlled through the Design table. Create several configuration and change these parameters in each one through the Design Table.

Artem Taturevich
CSWP

 

[tmox]

to answer your question directly.........there are several columns (parameters) that do not show up in the propery manager page.
I managed to get this file to work in the library and be selectable through property manager, however, i had to create a bogus sketch with a circle and 2 lines. I dimensioned the circle which gave me a dimension that the design table could "see" for the diameter and a dimension between the 2 lines for my length parameter. I then hid the sketch globally. I'm not happy about it,........but, it works fine. There should be a way to force a parameter. What if i wanted to sort between "finished" and "un-finished" or some other factor that cannot be shown in a sketch?
Now i am trying to get the material property to show up in the design table. I changed the material in a couple of different configurations so that the design table could automatically pick up on the parameter. This is not working for me.

 

[CorBlimeyLimey]

Perhaps if you can explain more what the Diameter and Length actually relates to, you might get more pertinent responses.

My first question is why aren't those dimensions in the model? Do they not relate to an actual feature? Are they raw material sizes for example?

As for the config material problem, that appears to be a limitation/bug/unfinished-function.

 

[tmox]

the part itself is a rivet which uses a revolved sketch. I dimensioned the diameter using a centerline, but, after the revolve the dimension was reduced in the sketch to a radius by SW. the length was never in the model. The finished length is not the purchased length. eg. i want to buy a 1/8 x 1" rivet, but the finished length (in my sketch) is only .88". But as i said above i was able to get that working using a bogus sketch.
What can i do about the material issue though?

 

[drawoh]

tmox,

You have a file with a hundred configurations, and you want to select by diameter and length. I betcha you want this thing to sort logically as well.

Use Excel to generate the configuration names. Let's assume you have diameters from 0.1" to 1.5", and lengths from .25" to 3.5".

Encoding decimal points in a configuration name is tricky. A nice code for a Ø.75"[×]1.25" long part would be "075x125"

First, name your columns. Definitely, name the DIAMETER and LENGTH columns, so that you can use these terms explicitly in your Excel equations.

Second, make sure the first column in your design table is formatted as "General". The default is to format it as text.

Here is your configuration name...

=IF(DIAMETER<1,"0","")&DIAMETER*100&"x"&IF(LENGTH<1,"0","")&LENGTH*100

You should be able to hack this to get exactly what you want.

JHG

 

[CorBlimeyLimey]

The diameter dimension can be fixed by re-dimensioning and placing it on the other side of the centreline, or maybe by clicking the diameter option in the Dimension Manager.

Also, if you are using a DT, you could simply double the referenced radius.

The DT is just an Excel spreadsheet; all the Excel functions are available to manipulate the model data. If the modelled size is shorter than the purchased part, you can use IF statements to select the correct purchased size.

 

[tmox]

I guess my question should have been " how to add a manageable property to design table".
I am ok with the diameter and length. What i want to know is when i add a property to the design table, how can i use that property as a filter.
The diameter and length are now dimensions in a bogus sketch so that when i use property manager it "sees" both of those and i can sort by those parameters.
I also have material in my DT but, that doesn't come up as an option in property manager.
HOW DO I SORT BY MATERIAL when i am not offered that column as a filter by property manager? Can i force this somehow??

 

[TheTick]

Usually I start by adding a config-specific property through the user interface. Then, when I edit the design table, the property shows up on the list of things I might want to add.

 

[drawoh]

tmox,

What do you mean by using a property as a filter?

You can add material as a property, ($PRP@MATERIAL). You can make the material show up in the configuration name. If you are selecting configurations at the assembly level, you are either going to have to use the SolidWorks tool, or you will have to write an API routine.

You can make the configuration names sort, making your search through hundreds of configurations simpler.

If you are selecting material and finish as well as length and diameter, you are going to have a lot of configurations. Perhaps you would be better off breaking this up into several files, and just vary one or two parameters. A file with a hundred configurations is a big file.

You can swap components within the assembly browser. This works seamlessly if the new component is a copy of the same model as the original file.

JHG

 

[tmox]

I tried the config specific property (TICK) and although it does show up on the spreadsheet when i run the configuration property manager i get the message, ' this file does not contain features that can be used with configuration property manager".
I am filling up the library. I DO NOT want to sort by configuration name. If the property is shown on a sketch it is easy to have those values become filters (dia. and length). Properties not found on the sketch are a different issue and the source of my problem.
for example i have a file with Mil-spec rivets. Diameters from .086 to .375, lengths from .125 - 3", materials include Aluminum, Aluminum Alloy, carbon steel, stainless steel, and copper. There could be 400 combinations.
If i was to use the filters i would select material, then diameter, then length.
On another part there are different materials, differing finishes, various panel sizes(thickness fits), and threads. None of these "filters" are dimensions in my sketches.
Please, please ........there has to be a way!!!

 

[drawoh]

tmox,

This sounds a lot like the SolidWorks toolbox.

If you are pulling a component out of a Windows directory and installing it, you select on configuration name. You create intelligent, sortable configuration names, and/or you use multiple files as I noted above.

How about you create configuration names out of all the parameters you select by, in logical order.

"BRONZE[&nbsp;]NICKPL[&nbsp;]0.125[&nbsp;]1.25"

Go through the list looking for bronze. Go through the bronze looking for nickel plate. Go through the nickel plate looking for Ø.125". Go through the Ø.125" looking for 1.25"[&nbsp;]length. This is very easy with a spreadsheet.

Your next choice is to create an API program for installing your parts. You should be able to extract configuration specific data, and provide a window for selecting the parameters you want. This requires you or someone you work with to write Visual Basic or C++.

JHG