I wanted to create a standard note that would list the material, hardness and finish of my part. To do so, I had two requirements. The first was to link the note to my part file in case my drawing was lost or corrupted. That way, the information would still reside in my part file. The other requirement was that if one of the three conditions did not apply, the note would be automatically renumbered and the extra note line removed.

Here’s how to create a standard drawing note that is linked to parameters in your part file.

1. Modify the start part to contain six text string parameters. In this example, they are called NOTE1, NOTE2, NOTE3, MATERIAL, HARDNESS and FINISH (Fig. 1).

Note that it is important to add the parameters to your part before adding the relations. If you don’t, you will get errors when you try to save your relations.

2. Add the following relations to the start part.

NOTE1= "1. MATERIAL: " + material

IF hardness == "NONE"

IF finish == "NONE"
NOTE2 = " "
ELSE
NOTE2 = "2. FINISH: " + finish
ENDIF

NOTE3= " "

ELSE

NOTE2 = "2. HARDNESS: " + hardness

IF finish == "NONE"
NOTE3 = " "
ELSE
NOTE3 = "3. FINISH: " + finish
ENDIF

ENDIF


3. Create and save a copy of your standard drawing note so you can reuse it in all your drawings. Here is the body of my standard note.

{0:NOTES:}
{1: }{2:&NOTE1}
{3: }{4:&NOTE2}
{5: }{6:&NOTE3}

4. When placed on the drawing, this is what your standard note will look like.
NOTES:
1. MATERIAL: A-2 TOOL STEEL
2. HARDNESS: Rc: 58-62
3. FINISH: BLACK OXIDE

Keep in mind that the part you are working with must be the “active” part in the drawing when you add the note.

Kenneth S. Johnson is an associate industrial engineer at ITT Industries, Engineered Process Solutions Group. He can be reached by email at Kenneth.Johnson@itt.com.