Tips for text

GD&T

• Use parametric GD&T when you can, and try this if you want to create a custom note.

Type this as the text:

And get this as the note:

• Notice that you type @[ before the symbol and then type @] after the symbol to create a box around it.

Superscript

Type this as the text:

25 ft@+2@#

And get this as the note:

Notice that @+ goes before the text to be superscripted, and @# goes after.

Subscript

Type this as the text:

C@-6@#H@-12@#O@-6@#

And get this as the note:

Notice that @- goes before the text to be subscripted, and @# goes after.

Multiple formats within single note

To edit the style of one section of a note, first click to select the entire note, then click again to select just the section you want to change. You can then RMB -> Text Style... and change size etc as required.

This works directly with separate lines within a note, but to change just one part within a line you must first separate that section by adding {1: and } around the relevant text:

{1:Large Text} Small Text

Separate Line

Then close the note editor and proceed as above.

To insert text symbol directly from the keyboard (text symbol as a font): press CTRL+A when in a Note Properties window.

To come back to standard font, press CTRL+B.

In the exemple below I typed "azertyuiop"

To round the value of a parameter called in a note, add [.X] after the parameter name, X being the number of decimals.

To see the result of a note change without closing the note window, simply click on your drawing's background when the changes are done.

It will act like a "Preview" button.

What was the trick for putting in your own dimension?

It has something to do with @D0 or something and then you type in your own dimension.

If you don't want to mess with pen tables and you export PDF drawings, try assigning "thickness" to your text.

I use .012 in in/lb (SAE) drawings providing nice crisp text in the PDF export.

Also, a nice font for distinguishing 1 (one) from I (upper case i) and l (lower case L) is ISO30985FONT. It is the closest thing I found to the Creo Direct Modeling default HP font.

I found this that might help this category:

Use a $ in relations to use negative values -

Relations All relations valid in a Creo Parametric model can be entered in a Pro/PROGRAM design. If an expression you want to include in the RELATIONS statement contains more than 80 characters, use a backslash (\) to interrupt the current line and continue the expression on the next line. The format can be as follows: RELATIONS PARAMETER = COVER_SIZE/2 + LENGTH*0.75 -\ 0.75*d3*d3 + THICKNESS*2 END RELATIONS

Changing the material density in a part causes the system to update the mp_density value in relations and vice versa.

• When using negative dimensions, a dollar sign ($) must precede the dimension symbol in both the input statement and the external input files. For example, use $d20 instead of d20. The dimensions will not be updated if a dollar sign does not precede the symbols.
• If the program assigns a value to a dimension variable that is already driven by a part or subassembly relation, two error messages appear. Edit or remove the program relation and regenerate.

Also found this:

If you have a string of variables like in hole callouts, you noticed that you require spaces between the end of the variable and new text characters. This is why you see...

&THREAD_SERIES - &THREAD_CLASS

UNF - 2B

But there is a little known method to remove the requirement for the space:

{0:&THREAD_SERIES}-{1:&THREAD_CLASS} ...which returns

UNF-2B

Old school editor but this is what makes it work.

Why didn't PTC do this for the hole CALLOUT_FORMAT?

PTC, are you listening? This is what "we" call fit and finish