Skip to main content
S
SolidPerks1-Visitor
1-Visitor
July 15, 2014
Question

Parameter Syntax - digging deeper

  • July 15, 2014
  • 3 replies
  • 7813 views

I suspect like many users, we have a Weight parameter set up to reference the mass properties. I discovered a syntax issue & I want to dig a little deeper, just because... I found it by trying to copy-paste the parameter callout from the note editor in one drawing to another drawing of a different model. The callout sytax was "&WEIGHT:5[.2] LB."

I understand that "&WEIGHT" calls the mass properties, "[.2]" controls the value to 2 decimal places, " LB." is descriptive text.

I realize, now, that the ":5" is system generated and refers to the model being referenced.

My questions is how do I confirm the model reference? Is the a RMB menu or property box somewhere in the tree or user interface that will tell me the model reference number?

In the case of a mutli-model drawing, I want to control the model parameter references, for template set-up, design automation, etc. The reasons for understanding & controling this bit of syntax are many. Thanks in advance for any help.


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

3 replies

D
dgschaefer21-Topaz II
21-Topaz II
July 15, 2014

The .5 is the session id. You can find it by going to the relations dialog and looking under the "Show" menu for the session id command. That's in WF4, they may have changed things a bit in Creo, but you should be able to find it in the relations dialog.

In a drawing, the session ID is not necessary. If it's a multi-model drawing, Creo will automatically add the session id for the current active model and will track it from then on.

Session IDs are assigned as parts & assemblies are retrieved. They are different with every session, as the name implies, and Creo / Proe seems to do a good job of tracking them from session to session.

T
TomU23-Emerald IV
23-Emerald IV
July 15, 2014

I know of two ways.

  1. Open an assembly. Go to "Tools", "Relations", "Show", "Session ID". Pick "Part" or "Assembly", then pick on one (part or assembly) in the model tree or on screen. The session ID will be show in the message bar.
  2. Add the text in the attached file to a note in a drawing. (courtesy of Mark Heinze - PTC User list)
S
SolidPerks1-VisitorAuthor
1-Visitor
July 15, 2014

OK, I understand what both of you are saying. This seems to be a type of memory management feature of Creo. If so, what purpose does it serve to the end user, other than stating an ID number? Is it used in upper-level design automation, or custom programming?

If the Session ID constantly changes, based on what is open and in what order, WHY does it show up in my text editor? It seems that unless it serves a purpose to the user, it should be 'hidden' somehow and not show-up in the UI.

Give this number some meaning... or should I just make a permanent mental note to ignore it?

Thanks for your help!! Even if I seem ungrateful, I do appreciate it, and I learned something today...

T
TomU23-Emerald IV
23-Emerald IV
July 15, 2014

Fundamentally you need some way to refer to other models in notes and relations. PTC could have simply displayed the file name, but that gets confusing when multiple files have the same name but different extensions (ex. parts and assemblies). If they simply hid the session ID, you would have no idea what that specific relation/parameter/dimension actually referred to. It also is similar to the syntax used to refer to feature level information: "<parameter/dimension>:FID_<feature ID>". Normally you won't need to worry about it unless you are creating relations or notes that need to refer to a specific model other than the one currently active.

Terms & ConditionsAccessibility statement