Happy New Year to all.
I have a problem I would like to fix. Sometimes I change the dimensions of a material I use but then I have to open Iproperties and change the description by hand. This can create problems as you can understand especially when I forget to update the Iproperties.
Then I had the thought to automate it. Lets take a steel bar as excempel. I have thickness and width as parameter, both are exported and available under IProperties/Custom. But they show as 200 mm and 10 mm. I would like to loose the units. I tried also UL but then it reads 200 ul and 10 ul.
What I like to get are just the numbers, no units. I like to use it to create this "steel bar 200x10" where the 200 and the 10 are linked to the Parameter and will change when I change the dimensions av the steel bar.
I do hope somebody can help me.
Greeting Toon Sol
Solved! Go to Solution.
Solved! by ccarreiras. See the answer in context.
Solved! by Namoi1. See the answer in context.
I think just right clicking on the exported parameter and choosing custom property format, and removing the check mark beside Units String would have been much simpler than Ilogic, but hey, up to you.
I'm have heard about iLogic but don't know enough about it to use it.
All help is welcome.
Check the part attached.
Go to the parameters chart and change the variables Ref1,2 and 3. The Part number will change accordingly.
You can use this part as a template to use it often.
It works as I had hoped and I understand the lines in iLogic.
But one more question. Ony suggestion how to add this line to standard steel forms in the library?
You can´t edit the standard parts within content center...
BUT, You can create your own library inside content center (copy standard parts and edit them) or create them and publish to your custom library. Doing this way you can use Frame generator with your profile parts.
If you want to use standard parts and have similar results, you can edit the "Part List" to achieve what you want.
ITS BETTER you explain what you want to do, what's your workflow, etc, because may exist different processes to do what you need.
I have now used your solution on parts that I have drawn myself and it work perfect.
But I would love to have the same result with "standard" materials coming from Content Center.
That restult being that if I change a dimension the text in Stock Number will change acourdingly.
Like i said, you can't edit cc members, unless you make your own library and then you can publish your parts with the iLogic code inside.
For cc parts, you can have similar results by using automatic variables inside the cc parts (Like G_L) to compose the part number in the Part List (in the drawing).
I do understand that with the parameter in a cc part i can create my own part number but that number is not dynamic.
It is created when you place the part from the cc in you assy. When you change a parameter afterward the part number will not change.
But thanks for all your help. It has given me a leg up.
You can place cc parts as standard parts, or as a custom part.
If you place the cc part as a custom part, the part will be save in your work folder and you can add/link the variables to the iLogic rule, and then, this cc placed part becomes associative, regarding the part name.
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