A few wIildfire questions

Hi All,

I have not used Pro/E in about 3 years (using I-DEAS and Solidworks)
and have just got a job using Wildfire 2.0.
I would have considered myself pretty knowledgeable on 2001 and have a
few questions as to functionality that I think is missing / can't find
/ Think I seen on wildfire demos.

Q1. 3D sections? Has this functionality been added yet?
Q2. Is it possible to extrude from a mid plane to 2 different surfaces
as the extrude extents? Can't seem to get this to work. On 2001 you had
the option of setting the extents of each side of the extrude from the
midplane - very handy functionality!!!!
Q3. I thought that they had added the ability to offset sketch entities
in the normal sketcher, Not just sheetmetal. Can't find it?
Q4. Why is there no ICON for a standard sweep. Am knowledgeable of the
VAR Sec (They did change the terminology) Not always want to sweep with
a tangent path. (Just a rant)
Q5. How do you get Autobuildz to work?
Q6. 3D annotation, Where are the menu's for it?
Q7. On 2001 I had a colour map file. When added to the config.pro every
time I started pro it loaded. This has been changed to an appearance
file. Have made one, how do I get it to load automatically? Is there a
config setting?
Q8. Working directory -- Has anyone else experienced, a) set your
working directory and b) open a file from another directory c) Start a
new part d) save the new part ---- and it saves to the directory you
have opened a file from in b. I have fixings library's set up using a
search.pro file and anytime I import a fixing and start a new part it
saves to the fixing directory. - Annoying.
Q9. I am having difficulty in setting up the new mass properties
relation. Can't get it to work.
Q10. What is the PTC common name??
Q11. Has there been any huge changes to the BOM functionality?

Overall I do like the new interface, have done the standard get up to
speed exercises.

I would appreciate it if anyone could help out with the above.

Regards

Steve

 

A few hours of reading thru Help will answer most of your questions. Some of
the easy (I might even know the answers) ones ...

Look at the Options pop-up

Use Edge tool flyout button for offsets

Add it to a toolbar (Tools, Customize Screen)

Not sure whatcha talkin about.

Insert, Datum, Annotation

Think pro_material_dir will fix you up.

Look at file_open_default_folder

Windchill related?

 

... Not always want to sweep with a tangent path. (Just a rant)

Ok, think I see (didn't know it was there, don't know what it's for). Start
VSS. Pick trajectory. Hold cursor over trajectory so preselect highlight color
shows again (cyan?). RMB for shortcut menu.

I don't know, never having used pre-WF, but gather that there have been changes
in the curve chains are built. Think there's even a (object selection
techniques?) tutorial on PTC's site. Might meander around the site for a while.
Think there is a customer resource section that has some stuff specifically
targeting those transitioning to WF.

 

Not sure what you mean by 3D sections. Often people mean what's called in Pro/e an
offset section. It's been there for a while.

What Jeff said

It's a flyout of an icon that looks like a corner of a box highlighted.

WJS, but don't think you can tailor options of a sweep within an icon, i.e., pick
an icon and it has your preferred options filled in. Also, whether icons are
available somewhat depends on progress toward their conversion to Dashboard
functionality. The converted stuff appears in a Menu bar menu with an icon next to
the text.

Set the config options autobuildz_enabled to YES. After that, I'm not sure.

WJS or pro_colormap_path which you can Browse to

WJS and set it to working directory

1) assign a meterial in 'Edit>Setup>Material' or at least set density
2) in 'Tools>Relations, create a relation something like Weight=pro_mp_mass. You
can confirm that these have values by going to the bottom, clicking the arrow for
Local Parameters. You should have created a parameter called Weight that'll be
listed in the local parameters and have a value assigned. If you want to see where
it got the value, click the dropdown list that says MAIN and you'll get Alt and
Report Mass Properties. Pro_mp_mass should be the first Reported mass prop and all
the rest should have the values you'd see if you ran Model Analysis.

Don't think anything's been added or improved in 10 years, although PTC's made a
faint stab at getting some OLE functionality with Access/Excel, but really crude,
rudimentary. The way they generally work, they put some teaser functionality in
the basic program then come up with an addon module that costs thousands extra
that has all the neat, really functional stuff in it.

 

Hi david

What I mean is to display an isometric, trimetric or perspective
section in the drawing.

I am aware of the offsetting of existing edges from solid or surface
geometry.
I thought I saw a demo when wildfire was going to be released that you
could select a chain of sketch entities and offset them. Something like
the
AutoCAD offset command. You didn't need existing geometry to offset.

Having been out of the Pro/E world for a few years, Does anyone know
when they plan
to have all the other functionality on the dashboard?

I have all that set up and still no luck. I never had any problems with
the old relation. I would say I am doing something stupid, and can't
figure out what. I am getting a relation error "Invalid data type
combination at right side of expression" This seems stupid as the
pro_mp_mass is at the right side of the expression. I have pro_mp_mass
in my reported mass properties at the top of the list. Can you post
pictures on this group? I took some screen dumps of the
relations/parameters dialog boxes.


Thanks for clearing these issues up for me.

Steve

 

Still clear as mud. Never heard of it. Maybe you could give a little more than a
superabbreviated, 12 word title to the manual describing what you're trying to do,
you know, at least some descriptive chapter headings. Maybe what it looks like,
where you've seen one before, how it was created, an interesting, entertaining
story for the poor dolts who work here. We're easily amused!! And we live for
facts and numbers. Ummm, numbers, precious numbers. We love any story with numbers
in it. Or, as the immortal Jerry McGuire put it: "Help us help you." Or as someone
from the early days of computing said: "Garbage in, garbage out (GIGO)", you get
what you pay for: you think not enough of your question, your dilemma to invest
some time in explaining it, you'll get as much in return.

Since Pro/e has substituted the sketch for the sketched curve, geometry created as
sketches can be used for a lot of stuff, including for sketch offset references.
So, you do a sketch of something, just planar sketched geometry. Then you want to
create a feature. You start an extrusion, pick the internal Placement icon and
Define. Pick some plane that's parallel to the sketch you just created and some
references. When you get into sketcher, do 'Offset entities', and pick the sketch
entities you just created. Sketches can be used the same as other geometry. Maybe
this is what you were thinking of.

I think they either have no plan or will drag it out to Slowburn 10 or
Barelyglowingember 20, however much milking the market will bear. They could have
done all this in one swell foop, when Wildfire was introduced, or some years
before that, when 20 started the current interface change. Now Dashboard is
getting mixed with "intermediate", modified Menu Manager functionality and new
'interfaces' are being introduced, as time goes on. Pro/e currently has about half
a dozen interfaces (including the keyboard entry one of a decade ago that still
accepts old style mapkeys) and no abatement in their creation. IOW, your guess is
as good as mine and PTC ain't sayin'. There are no more closely guarded secrets in
the world of government and industry than PTC's plans for Pro/e.

I think we could stand some pictures, unless someone thinks this might bring
USENET to its knees. But I wouldn't be surprised if USENET or your service
provider filtered it out. If that bombs, send them to me. I'll take a look.

 

Hi David,

Can you send me your e-mail address. I have a drawing done that will
explain the 3D section in complete detail. I can then send you the
weight issue pics as well.

Thought the weight relation may have been something I carried over in
my 2001 start part. So tried to set it up completely from scratch in
wildfire. Didn't work either. If you can send me your e-mail address,
or send a blank mail to "sfarrell169<nospam>@yahoo.com" I can reply to
you.

Thanks

Steve

 

Hi David,

What I had done in the past was create a map key to close a model / drawing in
pro/e. The map key would regen the model, calculate mass properties, regen again
(this would update the weight), and close the model. This ment that any time you
opened the model the correct weight would be displayed. This does however not work
with wildfire. I think adding the analysis feature is the way forward. I have
created the analysis feature and called it MASS_PROPERTIES. Set the mass create
yes in the result param and regen request to always. Used the relation
WEIGHT=MASS:FID_MASS_PROPERTIES. This works but doesn't seem to update
automatically when the geometry changes. If I go to window activate it then
updates. Is there a variable somewhere to tell Pro/e to always update parameters?

On the 3d section view, No worries worked a treat. The red X was putting me off I
think. Didn't think it would work so didn't try. A lesson I learned many years ago
but forgot when dealing with PTC.

Thanks a lot for your help.

Steve

On relations question, this is pretty easy. You're at the point of having done
everything right and are about to create a relationship to capture a mass property
calculation so it can be reported in a parametric note. So, in relations, you do
wate=pro_mp_mass and it bombs, tells you something's wrong. The problem is this:
there's nothing to report as a value of pro_mp_mass. For some reason, PTC's
decided not to fill this system parameter with a value upon its first being
referenced or even, automatically, upon geometry being created and the part
regenerated. Instead, you've got this special, cute, secret, cultish hoop (only
the real insiders know about this one: dumbass trivia to separate the "men" from
the "boys", IOW, a program written by juveniles) to jump through. Back in
'Edit>Setup', go to Mass Props and at the bottom, click Generate Report. This
stupid thing triggers the filling of a bunch of parameters with values. The worst
of this is that it's reactive and only holds/reports the values from the last such
report gen. It is possible (haven't confirmed this) that going to the bottom where
is says Initial and setting this to Post Regen will make it more current. Problem
is, even when it does this, it's telling you the value, not from this regen, but
what it picked up but didn't show in the wate variable at the LAST regen. IOW,
it's always a regen behind. Forget this method and do Analysis features
('Insert>Model Datum>Analysis') and move them to the Footer which makes their
value always current.

David Janes
----- Original Message -----
From: stephen farrrell
To: David Janes
Sent: Tuesday, February 07, 2006 6:37 AM
Subject: Re: A few wIildfire questions


Hi David,

Thanks for the mail. Pictures attached.

Steve

For the email address, just remooge the munging at the end. I'll take a look
this evening.
David Janes
----- Original Message -----
From: yomoto
Newsgroups: comp.cad.pro-engineer
Sent: Tuesday, February 07, 2006 3:15 AM
Subject: Re: A few wIildfire questions


Hi David,

Can you send me your e-mail address. I have a drawing done that will
explain the 3D section in complete detail. I can then send you the
weight issue pics as well.

Thought the weight relation may have been something I carried over in
my 2001 start part. So tried to set it up completely from scratch in
wildfire. Didn't work either. If you can send me your e-mail address,
or send a blank mail to "sfarrell169<nospam>@yahoo.com" I can reply to
you.

Thanks

Steve



----------------------------------------------------------------------------