hi i have a problem, i have a template in fraction, but i need thickness property in decimal number
Sheet metal "thickness" is a global variable created and assigned a value when you create a base flange and the "Sheet Metal" item is created in the tree.
So, are you're using SW sheet metal features (and the "thickness" global variable it creates)?
Or are you forcing your sheet metal features to a "thickness" property created independent of the sheet metal feature?.
What is the red circled drawing note linked to?
How is the part's "thickness" global variable shown in the equations dialog (Tools>Equations)?
As a fraction?
As a decimal?
Post a screen shot of your equations dialog (at least the top portion of it).
I would hope it is a decimal since calculations are made on this value.
If fractional, the thickness calculations will be off due to rounding from the 4 decimal place gauge thickness.
If the "thickness" global variable is decimal, create a custom property (can't be the same name as any global variable) and equate the property to the thickness global variable.
Link the drawing note to this property (which is in the part file).
That value is displaying as a fraction because that's what you have Units set to at Tools > Options > Document Properties > Units. If you'll change that to decimal the note value should display as decimal. That will also cause your dimensions on the drawing views to display as decimal, but it's easy enough to override one of them, save that as a Style, and apply it to all of them. How do I change my units from inches to mm (or vice versa)? may be of some help.
The property is a text string literal equal to the thickness (which appears to be in mm) and is quoted when linked in a note (as shown in my PDF).
Notes don't have the fractional options of dimensions (that I know of).
This is why I asked above, what the drawing thickness text was linked to.
If a thickness dimension was clicked on during the editing of the note, then yes, the fractional value will be in the note.
But a note directly linked to the part's THICKNESS property should quote what the property evaluates to.
I think editing the drawing note to directly link to the part's THICKNESS property will remedy this:
It's easy to try without modifying your title block (yet).
Just create a note on the drawing as I did and link as shown above.
What is displayed? Decimal? Or fraction?
Retrieving data ...