text driven by multiple parameters on a solid model

[bp]

I would like to add a text on my gear (solid part) using data from my parameters.

Normally I would write: "Mod &m, &z teeth" refering to my parameters with the "&".

Sadly the text line does not accept this.

Any suggestions?

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[John.Pryal]

Hi, split the note up into 4 elements within the one feature. First bit, would be manually entered text "mod", constrain/dimension it, next bit would be use parameter, select your parameter "M", constrain/dimension it, relative to the "mod" text. Repeat the procedure, for number of teeth text. Hopefully, this makes sense to you.

Hopefully, i have understood your problem.

John

[bp]

Thanks,

It makes sense, I was just hoping there would be an easier way..

for example, is there a way to make a new parameter which contains the combined text and use this?

[John.Pryal]

How about you make the value of a single parameter read (string) "mod 3 118 teeth". Not quite ideal, but its a work around.

John

[VladimirPalffy]

Here is the short tutorial for you How to create a parametric 3D text in PTC Creo Parametric

Regards,

Vladimir

[JonathanHodgson · Accepted solution]

You could use a relation to generate a string parameter, converting the numbers to strings within it.

I think it would be something like:

label = "Mod " + itos(m) + ", " + itos(z) + " teeth"

and then choose the 'label' parameter for your text, as already shown.

This gets a little more tricky if m is not an integer - this has been covered elsewhere though.

[bp]

Works like a charm, thanx!

[Patriot_1776]

Note: You can also string together string parameters as well, like this:

PART_NUMBER = DRAWING_NUMBER + DASH_NO

NOMENCLATURE = DESCRIPTION1 + SPACE + SIZE

MATERIAL = ASMSPEC1 + SPACE + ASMSPEC2

So, I'm sure you can also string together any combination of integer and string parameters to get what you want.