ProE Tree Column refresh/regenerate

Hi everyone-

What I have done is create relations and then display several of the
parameters in tree columns. The problem is that when I change the values of
the parameters, they do not automatically update in the main window
(sometimes they update if you change it more than once, but it is
unpredictable).

If you don't know what I'm talking about: under the 'Settings' tab in the
ProE interface, there is a selection 'Tree Columns', which allows you to add
columns to the layer structure window, such as Model Parameters. I am using
Wildfire 2.0 M120.

I am new to this newsgroup so if there is a post or guideline on etiquette,
please point me to it- thank you! If you cannot tell, I am also pretty new
to Pro Engineer

sincerely,
David Garber
PTP / 24-E150

 

Dave,

I don't have an answer for you. This newsgroup is pretty dead though.


Try either

http://www.ptcuser.org and the email exploder (prouser group)

or

http://www.mcadcentral.com and the ProE forum.

Good Luck!

 

We ain't dead, just a little sleepy. Peter's suggestion is a good one, though.

Are you regenerating the part(s) and / or assembly? I'm never sure when
something needs regen'g or not (there's an indicator on the status bar but I
never remember to look at it) so when in doubt....

It might be noted that Pro/E will every now and then fuss about regen'g. Model
Player or just RMB / Edit Definitiion / OK some early model feature will force
it to wake up.

 

Welcome, David Garber, to this dead group.

Based upon your description (changed a paramter value, didn't update model), I'd
agree with Jeff. Editing parameters in relations is like double clicking a feature
on the model, getting the dimensions to show and changing one. If it's a sketched
section dimension, you'll see the internal sketch change size, but the part does
not automatically change; you have to do 'Edit>Regenerate' or hit the regen icon.

As far as participation goes, I personally appreciate people giving some detail of
their problem in the question, including such things as the rev of Pro/e people
are using, what you are trying to accomplish, not just what buttons you pushed.
Present enough breadth and depth of detail that we get enough of the picture so
that we can help you. The best answers need the best questions.

David Janes

 

is what you are changing tied to a piece of geometry?
unless a regen occurs due to a geometry change proe
doesn't hit the rel table..least that has been my understanding

parameters yes..relations only if you force a regen

also I concure on mcad and ptcuser..moves a little faster there
than here

 

Thanks for the advice on the board- I will be sure to try those 'more
lively' boards as well.

Ok, a better explanation of what I am trying to do: I have a simple disk,
with 3 holes poked in it. I want to check and display that the distance
between the holes and between the holes and the edge of the disk is above
some minimum thickness. I measured the distances between the holes and made
these feature parameters, then used the relations window to do comparision
(if dim1 <= minthickness & dim2 <= minthickness & dim3 <= minthickness.... I
then display a boolean value for this, as well as each of the individual
thickness values).

Everything you guys said is true-

cad/cam/guy: what I have been doing is changing the value for
"Minimum_Thickness", but since this is not tied to the geometry,
regenerating the model does not update the relations. With
"Minimum_Thickness" defined as a parameter and not in a relation statement,
it does update instantly. However, all of other values do not update since
they are defined as relations.

Jeff Howard: I tried redefining an earlier feature, and you are right, ProE
then does regenerate all the values I am trying to display.

The idea of displaying this information was to make it easy to see if the
model satisfies design requirements (this is a launch tube, and the minimum
thickness is the thickness required between separate missiles for
pads/support/etc.). Do you guys have any suggestion for an easier or more
effective way to display this information?

thanks again,
David

 

I should have said this at the start- all I want to do is "output" or "write
out" information for the user to see (i.e. does the model satisfy the
minimum thickness requirement? YES or NO). Displaying it in a model tree
column was the best thing I found. But if you know of another way to do
this, I would love to hear it ;-)

 

The idea of displaying this information was to

Not sure if this is something you'd want or not; a 3D annotation in the form of
a driven dim or note referencing an existing dim or parameter, datum evaluate
feature (I think they have their own set of regen / update problems), ....

 

Yeah, you're right ~ it's very nice to see constantly updated values in the model
tree. The new thing in WF2 is the 'footer' and the ability to move parameters,
especially those that should update after a regen, into the 'footer'. Analysis
features ('Insert>Model Datum>Analysis') which can capture a measure, such as you
are trying to do, into an appropriate parameter, are a prime candidate. You could
also, if you wanted to get really fancy, create a parameter, such as TOO_THIN, as
a YES/NO parameter, set it to a default of NO, then do a relation which constantly
evaluated your DISTANCE parameter (created by the analysis feature) and when it
passed a trigger value, changed the TOO_THIN parameter to YES. So your model tree
could have the raw number of the DISTANCE parameter, plus the YES/NO evaluation in
a column called Too_thin. While you were in the NO values, you'd be golden; then,
you'd have to keep an eye out for just a shift to YES, which would set off bells,
whistles and sirens.

Doesn't seem undoable to me.

 

I think I have done what you said, but the model is not regenerating the
parameters in the model tree columns even when I change the geometry of the
part.

I created a feature parameter ('DISTANCE', distance between two of the
holes) and moved it to the regeneration footer. Although feature parameters
is an option under the model tree columns window, I do not see my feature
parameter displayed there...

I have a model parameter equivalent to "TOO_THIN"; in the relations window I
have:

X = DISTANCE - (Radius of Hole 1) - (Radius of Hole 2)
IF X < MIN_THICKNESS
TOO_THIN = YES
ELSE
TOO_THIN = NO
ENDIF

'MIN_THICKNESS' is a user defined parameter. When I change the geometry of
the part and regenrate the model, 'X' and 'TOO_THIN' do not update in the
model tree columns. I guess it is not reevaluating the relations when I
regenerate? But I don't know why. (as was mentioned before, going to 'Edit
Definition' of a feature causes a full regeration including these
parameters).

 

you can create a curve and tie its values to your model tree parameter,

my_curv_len=tree_value.. what ever naming scheme you are using
hide the curve and when you change the tree value.. geometry will
change
forcing a regen and running the rel table

i'd get away from using proe's names such as d1,d2,d3, etc and go ahead
and
name them ..with a name that means something will make it
a little easier to follow

steal from peter < the geo parameters > to pay paul <force the regen>