Associative notes and decimal point formatting 2

[hoyle]

Help
I require a note on a drawing to be fully associative with the model. I can do this with a named variable in the model, exposing the variable in the variable table, and calling up the variable in the label via the property text button. It works, and follows the model exactly.
My problem is that the format of the dimension is always to 2 decimal places, and I only want to have the numbers as no decimal places.
i.e.
" ON 99 PCD "
Instead of
" ON 99.00mm PCD "
Our support people say it’s just the way it is in Solid Edge, and there is no way out of it.

 

[beachcomber]

After a quick test it appears that the property text gets the number of dp's from File>Properties>Units>LengthReadout>Precision setting of the part file.
I just set this to 1 (ie. 0 dp's) and the property text rounded off the same, which is logical in a way.
I tried using the /@n qualifier in the property text but that had no effect (n is the number of dp's you want to display).
The only other way I can think of is to just place a dimension to the PCD in the normal way.

bc

 

[m4rc]

Hi,

To remove the 'mm' from the label you need to do the following... although it removes the label for everything.

Tools -> Option -> General, then uncheck the 'Show units in value field'

M

 

[hoyle]

Hello
Thanks for your help
After 7 years of being fully associative and Pro/e'd up, I suppose I shouldn't expect too much from this "also ran"

 

[KENAT]

hoyle, really?

SE isn't perfect but trashing it like that isn't going to encourage anyone to help you out much.

KENAT, probably the least qualified checker you'll ever meet...

 

[beachcomber]

Well said Kenat.
We can all find faults in ANY system, but that's not the idea of this forum.

bc

 

[m4rc]

Ah well, you get people from time to time that you no longer help in forums... seems this bloke does not 'think outside the box' just like he say people moving from a shopfloor environment cannot. I think he's too quick to judge people and programs... but maybe I'm too quick to judge him after reading two posts? Nah.

http://www.eng-tips.com/viewthread.cfm?qid=6376

(at the bottom)

M
Solid Edge V19 (and loving it)

 

[donyoung]

Hi,

to get rid of the unit label has nothing to do with 'not
being associative'

BC:

the /@n or /NU works only on *numeric* variables but unfor-
tunately SE exposes a variable always as text with unit
label. There is, however a neat trick to circumvent which
also removes the unit label:

- define a variable with type 'scalar'
- set the formula to the variable one would like to have
without the unit label
- expose *that* variable

now the /@n will work and the unit label is gone

See also SE Help --> 'Create Property Text'

dy

 

[beachcomber]

Hi Don,
Just thought I'd try this, but I still can't get the /@n to work.
I've created a scalar type variable in my part file and set its formula to the variable whose value I want to show in my draft file. The scalar variable is exposed.
Then in the draft I use the scalar variable in my call-out and add /@1 , but it still shows the number of dp's from the part file.
I'm using v19 - is it different in v20?
To be honest, I would normally create a bolt-circle and add a dimension to that.

bc

 

[donyoung]

BC,

your assumption is correct: it does work in V20 (I've V19
no longer installed)

dy

 

[beachcomber]

m4rc,
That was an OLD post, how on earth did you dig that out !!
It must be about 7 years since it was posted - mmmmm 7 years, now where did I see that mentioned ?

As for people coming off the shop floor, it's my experience that their knowlege is invaluable. I worked with a guy that had been on welding for a few years and it was great to know exactly what could and couldn't be done, assembly sequencing etc. Design isn't always about new ideas is it.

bc

 

[m4rc]

Hey, that's easy, all you have to do is click on the persons name and you get some info... then you click on the number of posts and you get -

http://www.eng-tips.com/userthreadparticipate.cfm?pid=562&handle=beachcomber

To be honest I just clicked on one of the posts and found that the comment was quite entertaining... didn't look at the date.

I've always found too that shopfloor colleagues are a wealth of information. Installation Engineers are too, they're the ones that fit it, so asking them a few simple questions can make their life easier and possibly yours too!

 

[donyoung]

BC,

update on topic 'decimal places'. In V20 they have
changed it in a way that also variables defined
within Custom as text can be used with @/n. the value must,
however start with a numeric part (leading spaces
will be ignored). Sample

Var1 holds 3.2 mm --> %{Var1/@0|R1} = 3 mm
Var2 holds AB 3.22 mm --> %{Var2/@0|R1} = AB 3.22 mm

/NU does not work that way maybe something for V21 ??

dy

 

[beachcomber]

Thanks Don,
I'll remember that for future use - when I get back on Solid Edge !
I'm doing 2D drafting at the moment using MIcrostation.
I can't believe how frustrating 2D is when you are used to 3D modelling. The best thing is, this is part of a world-wide company and their main system is Catia. The department I am in insist on retaining their 2D Microstation roots, so they have even gone as far as converting Catia drawings to dxf then dgn so they can use them
Hope to be back on Edge in the next week or two

bc