Associative notes and decimal point formatting

[hoyle]

On reading the threads, I notice others have had the same problems with this. here's my work around.

The problem = a drawing exists which has a note on it. It is required for the note to be associative and show the units in their appropriate formats.
WHAT WAS HAPPENING?
2.00 holes on 316.000 PCD
WHAT WAS REQUIRED?
2 holes on 316 PCD

The work round

The number of holes
Go into the part, and go to Tools/Variables/Variables.
Find the variable which drives the number of holes in the pattern. This will be called V123 or similar. Create another variable - just click on the next free cell, and type in OUTERBOLTPCD or another easy to remember name. Make this SCALAR, and make it equal to V123, by typing “ = V123 “in the Formula column.
Make sure you click the tick box to yes for the “exposed variable” option.(I think there's a quicker way than this....)
Close out of the variable table functionality, and back in to Part.
Go to File/file properties/Units/advanced units/scalar. Make this equal to 0 decimal places. OK, OK back to the part. SAVE.
In your drawing note with the hole call out command.
On the general Tab, click on the Property Text icon, and this time click on the Named Reference option, somewhere down the list will be a variable called OUTERBOLTPCD, click on this, and click Select, and then OK back to the General tab in the note command.
This will now be displayed correctly.

Now the PCD
Stick another view off the drawing sheet (so it doesn’t print), AND stick the centre lines in from the bolt circle command.
Smart Dimension this PCD circle, double click the dimension, it will be called V12345 or some such.
Go into the note with the hole call out command, and use the Property Text icon, click on the Named Variable Document, there will be a list with V12345 on it.
Click on that, and then click on the select button. This will put the value in the note.
OK out of there, and the note will be in the same dimension format as what is on the scrap view off the sheet.
DONE

I must admit it’s a long work around, and if you have lots of Patterned holes on lots of PCD’s it looses its novelty value.
If anyone has a better answer, please share it.

 

[donyoung]

Hi,

longish but OK ;-)

At least in V20 you can do it as follows (the value must
start with a digit):

- expose your variable, name it to say MyTest
- in draft do this: %{MyTest/@0|R1}

whereby /@n specifies the number of decimal places
you want. The above will strip them off @/0

Unfortunately one can't use the sitch /NU to get rid
of any units labels

For other modifiers see SE's help topic 'Create property text'

dy

 

[beachcomber]

For the PCD, how about dimensioning the pattern circle in the model.
Expose the variable for the dimension, then reference it in the note along with the number of holes.
The /@n doesn't work in V19, must have been changed at V20.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[beachcomber]

Also found that whatever value I use for /@n, it always rounds to 0dp. Has anyone else noticed this or am I doing it wrong ?

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[donyoung]

BC,

checked it with V20/SP5 and it did work:

myvar = 7,23

%{myvar/@2|R1} = 7,23
%{myvar/@1|R1} = 7,2
%{myvar/@0|R1} = 7

dy

 

[beachcomber]

Thanks Don, I'll try it again next week when I'm back at work.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.