Adding Smart Labels to Parts Using a Design Table
Using the Configuration Properties to Drive the Dimensions and the Label of a part through a Design Table.
Model Found:
Rotary Ring, For Tutorial
Video walkthrough available at:
https://youtu.be/PtQl_28Jlqk
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Step 1: Setting the Dimension to have Names
We want to change the Dimension Names to make them Easier to find Later on
First Edit the Sketch
Select the dimension to be change. If the Property table doesn't come up, Grab the dimension and drag it up or down slightly
Change the Name for D1@Sketch1 to ID@Sketch1. Continue this for all the dims you want to control
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Step 2: Adding in Configuration Properties
Open the Properties Pop Up:
Enter in the **Configuration Properties** that you'll want to control:
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Step 3: Creating a Design Table
Insert a Design Table:
Allow it to Auto-Create:
Add the Dims to the Table:
If Table Opens, Close it and Go to the Configuration Nav Panel, Select the New Design table and "Edit it in New Window"
Select the Properties to add to the Table:
The Excel should open. Select all data and change the Format to "Number" so you can use formulas:
Reorder/Format the table to match your preferences. Then In both the Description and the First column (Configuration Name) add Code in This:
="Ring OD: "&TEXT(<OD Column>,"0.000")&", Ring ID: "&TEXT(<ID Column>,"0.000")&", Cir: "&TEXT(<OD*pi() or Cir Column if you programmed it>,"0.000")
This is adding a bunch if string together to make the Test I want to see. This is explained in the video version in depth:
Add The Rows and Values wanted, this will make a lot of configuration for the part:
Save and Close. The Configurations will be added to the Configuration List:
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Step 4: Linking the Property to the Label
Add a sketch in the location of the label:
Select the Link Box to open the properties pop up:
Then select the Configuration Name:
Exit the sketch and the Text Label should now update with the Configuration:
