Newby questions

Greetings list, I'm trying to self-learn WF2. I know that I should do formal training but it's not convenient at this time. So the follow question are the questions
that I would ask in a class. You're indulgence and help is appreciated. Note that I have purchased and done the exercises in Toogood's Tutorials (WF1).
The following list is not questions but conclusions which I believe to be true, please advise if I'm in error: 1. one cannot apply a taper or draft angle directly during an extrude, either protrusion or cut 2. one cannot suppress an individual occurrence or otherwise modify a single occurrence of a pattern 3. the template file for mmns_part_solid is the same as solid_part_mmns (etc) 4. WF2 is not multi-threaded
The following are in fact questions: 1. How does one make changes to system colors stick, specifically the background for sketching. If it's in config.pro, it's pretty obscure or is there a way to automatically open a SCL file? 2. In a drw, when creating a section view I don't get the cutline arrows. I can show view direction arrows but they have the projection plane nomenclature not the section name 3. Is there a zoom "previous" 4. When doing a mmb orbit or spin, there is a red line centered at the spin center, what is it trying to tell me? It's movement seems much too random to be of any benefit 5. File>erase items not displayed What are these items, what should I know about them, how can I use them, if at all?
Thanks for any and all responses, BF
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Give us some background so we have an idea of where you are coming from with your observations/conclusions and questions. Conclusions: 1. Sounds like you have a UG background as UG can do those things at extrude time. 2. Again, UG can, Pro/E cannot. 3. That could be, The default is picked up from a config.pro setting. 4. Pro/E does not take advantage of multi-processor systems.
Questions: 1. config.pro setting to open a default .scl file. I think it has a new name in WF2. 3. No 4. It is the point that the spinning is being done around. That's it. 5. pro/E keeps everything in memory. When you do a File-Close, you haven't erased the part from memory. File -Erase will erase it from the system memory. S* files are your sketches used for your extrudes/protrusions.
--
Ben


"BF" < snipped-for-privacy@fakeyahoo.com> wrote in message
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Thanks Ben, I appreciate the answers / confirmation. My background is limited UG, but a wee bit. Mostly the midrange modelers, Solidworks, Inventor, Mechanical Desktop, Ironcad, Rhino and a bit of Vellum. Since you were kind enough to answer, I'll ask if you can give a bit further info on how to direct config.pro to open the .scl file? Also, does config.pro set the session's working directory and the model tree "tree filter settings" in the navigation tab? And while I'm here, is there anyway to change a copied part edge to construction or reference? Doesn't appear to be but maybe I'm missing something. And one last for now, is there any place to set or "play with" the graphics setting to try to improve the displayed render mesh? Again thanks for any and all advise, BH

but
questions
(WF1).
be
is
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random
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: Greetings list, : I'm trying to self-learn WF2. I know that I should do formal training but : it's not convenient at this time. So the follow question are the questions : that I would ask in a class. You're indulgence and help is appreciated. Note : that I have purchased and done the exercises in : Toogood's Tutorials (WF1). : : The following list is not questions but conclusions which I believe to be : true, please advise if I'm in error: : 1. one cannot apply a taper or draft angle directly during an extrude, : either protrusion or cut
True
: 2. one cannot suppress an individual occurrence or otherwise modify a single : occurrence of a pattern
Not true
: 3. the template file for mmns_part_solid is the same as solid_part_mmns : (etc)
No idea what you're talking about: check <loadpoint>/templates for all the 'default' templates Pro/e comes with and which can be referred to in config.pro options TEMPLATE_something. As to what distinguishes these templates, you will either have to get hold of a file utility which does a byte-by-byte comparison (Beyond Compare comes to mind) or open them as files and check out such stuff as parameters, units, material assignments, anything in the 'Edit>Setup' menu for differences. Also check preset views and layers for similarity/difference. Parts used as templates may be named anything and be stored anywhere; they are not marked as special in any way. So your solid_part_mmns could simply be a copy of mmns_part_solid and for no more reason than that somone thought this made more sense or just plain liked it better.
: 4. WF2 is not multi-threaded
First of all, four executables open to load Pro/e: xtop.exe, pro_com_message.exe, nmsd.exe and pglclock.exe. Pro_comm_msg reports 2 threads in the XP Task Manager Process Report; xtop reports 15 threads, nmsd is reported to be using 2. Seems to be multi-threaded though don't know what criteria you're using to judge this. Possibly rumors on the SW newsgroup? : : : The following are in fact questions: : 1. How does one make changes to system colors stick, specifically the : background for sketching. If it's in config.pro, it's pretty obscure or is : there a way to automatically open a SCL file?
Point to your custom system colors file with the config.pro option SYSTEM_COLORS_FILE and browse to its location. Then press 'Add/Change' and 'Apply'. If you don't do this, the changes don't take effect. Then make sure you go to the config.pro file menu (double disks at top) and save your changes to the config.pro file. It should be the config.pro saved in the initial Windows 'Start in' directory. This is where config.pro, config.win, tree.cfg, syscol.scl, color.map, color.dmt, layer.pro, and .dtl files should be stored so that they are found and load automatically. Some config.pro options let you specify different places to store many of these files. If there is no general pointer to a default file, any such file found in a set working directory will be used. You can have sets of these, say different ones for each project you work on, in each working directory you use. Pro/e is freighteningly infinitely configurable.
: 2. In a drw, when creating a section view I don't get the cutline arrows. I : can show view direction arrows but they have the projection plane : nomenclature not the section name
Possibly because you didn't give the section a name. To be safe and precise, make your sections in the model, give them explicit names and these will be selectable when you create section views in a drawing. Pro/e leaves such things up to you and makes very few assumptions for you.
: 3. Is there a zoom "previous"
'View>Orientation>Previous' is as close as you can get with Pro/e; no short cut that I know of, make Mapkey to simplify.
: 4. When doing a mmb orbit or spin, there is a red line centered at the spin : center, what is it trying to tell me? It's movement seems much too random to : be of any benefit
More control is available, as of Wildfire, by turning off Spin Center. It can be set to off by default in config.pro with SPIN_CENTER_DISPLAY set to NO. The new method in Pro/e, with spin center turned off, is to use the entity, feature or point in space by your mouse pointer as the center of rotation of the model. This point is moveable just by moving the pointer over another area of the model. Prehighlighting shows you what will be used for rotation or zoom focus.
: 5. File>erase items not displayed What are these items, what should I know : about them, how can I use them, if at all?
Unlike Windows programs where closing a document means erasing it from memory, Pro/e's close window just gets is more like the typical Windows Minimize window. It's in memory, but in the background. Opening an assembly effectively opens the models but they are 'opened' minimized ~ in memory but not the active part. In an assembly, they are accessible and available but not active. When you hover the cursor over the assembly, components prehighlight. With one prehighlighted, you can RMB 'Open'. Then the model moves to active memory. After making your changes, you can save and close the part file but it is still in memory, but not the forward, active memory. To see that it is still in memory, check the assembly and see that the changes you made are now reflected in the assembly component. If you close the assembly but don't erase it, it and all its parts/components are still in memory. If you select 'Open' and get a file list, supposedly of a disk directory, and pick a file that is already in memory, you may think you are opening the file from the disk but, in reality, you are 'opening' the one in memory. To purge memory completely of any and all opened files, select 'File>Erase>Not displayed'. Only then may you open the file on disk and only on disk.
David Janes
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Note
I agree with David Janes' response to your questions. But there is a way in Pro/ENGINEER to add a taper or draft to an extruded Protrusion or Cut feature. The functionality is called Draft Offset. You could even do this in several releases prior to Wildfire 1 and 2. Instead of using the Extrude icon in Wildfire, or the Insert-Protrusion/Cut functionality in Releases 2001 and prior, use the Draft Offset command. I'm at home now and can't remember the exact command sequence(e.g. Insert-Advanced-Draft Offset--or something like that). At any rate, you will still select a sketching plane, create a sketch, and enter an extrusion depth. A positive value with result in a Protrusion-like feature, and a negative value will remove solid material similar to a Cut feature. You'll have the opportunity to enter a draft/taper angle, and you can also have the software to add tangent radii to the top and bottom of the tapered sides if that's what you desire. It's not exactly as smooth as UG's functionality for this type of feature creation, but it will work in many cases. If you find that accessing the Draft Offset functionality requires too many menu picks, you could create a Mapkey and corresponding toolbar button for easy access to it.
Best regards,
J. Perry
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Thanks David and J.Perry, A much better and more detailed response than I had even hoped for much less expected. With regard multi threading, I was referring to multiple processors or hyper threaded processor, not really important either way. I don't recall Solidworks multi threading to different processors either, have to check sometime. I will have to check out the Advanced-Draft option, since most of my design is in plastics. The one thing that was not explained was how it is possible to make a single instance of a pattern independent? IE, suppress, delete or change without effecting the pattern as a whole. Thanks again, I think I'm actually starting to get some of it. BF
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: Thanks David and J.Perry, : A much better and more detailed response than I had even hoped for much less : expected. : With regard multi threading, I was referring to multiple processors
Pro/e is capable of utilizing the power of multiple processors with a config.pro option called PROCESSORS_TO_USE set to the number available and supported by your operating system. Obviously, if your OS doesn't support multiple processors, neither can Pro/e.
: I will have to check out the Advanced-Draft option, since most of my design : is in plastics. : The one thing that was not explained was how it is possible to make a single : instance of a pattern independent? IE, suppress, delete or change without : effecting the pattern as a whole.
Sorry for the abreviated answer, but when questions are vague, general, broad, the answers will be short and non-specific. Better answers require better questions. So, have you actually tried WF2 patterning? Seems that, with both a fill pattern and dimension driven pattern, it shows you instance positions. If you click on the black dot, it skips regenerating these. If you want them back, you edit definition and click them so they turn black again. Pretty simple, about as simple as SW!
: Thanks again, I think I'm actually starting to get some of it.
Shouldn't take you that long since you're a newbie to Pro/e, but not to the general concept, outlook and methodology of solids modelling.
David Janes
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Hi, David. Is there any documentation on this? I couldn't find anything on it. Unix only? Distrubuted computing has to be set up (it it's an optional setup during intall I probably skipped it)?
To go off on a tangent: Re Distributed Computing in the Installation Guide there is a statement; "Distributed Computing is suitable only for multiobject design studies.". What does that mean in English?
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:> PROCESSORS_TO_USE : : Hi, David. : Is there any documentation on this? I couldn't find anything on it. Unix : only? Distrubuted computing has to be set up (it it's an optional setup : during intall I probably skipped it)? : Well, I just checked WF2 and this is not even a config option anymore! Where I was it though was on a dual Zeon processor system with Wildfire on Win2k. Use of the second processor, according to the Task Manager performance graphs seemed to improve. Though, of course, this is anecdotal and could be completely coincidental that performance seemed sluggish to begin with. It could just as easily have been a network or licensing issue. But I wasn't the one who installed the software for a multiprocessor machine so I don't know if there was any special detection/support option offered or if got installed automatically. I would think it would be automatic. I mean who would buy a dual processor system then tell Pro/e NOT to dig into its bag of tricks to get whatever benefit it could out of it.
: To go off on a tangent: Re Distributed Computing in the Installation Guide : there is a statement; "Distributed Computing is suitable only for : multiobject design studies.". What does that mean in English? : MODS refers to an advanced function within Behavioral Modelling which varies and tracks the results of changing various model parameters on 2 or more different design goals and converges on solutions which satisfy all of them. But, when confronted with explaining similarities/differences between multiprocessor, parallel computing and distributed computing, it's not failure of the language to express but my lack of a degree in computer science that's holding me back. I am pretty sure that distributed computing is a somewhat different animal from dual processors, first requiring a program to be written with it in mind and second a computer architectures and high speed network that can handle keeping hundreds of processors working together. But this is stuff out of Scientific American and Fermi News, from Fermi Lab, where they have that kind of setup for data acquisition and analysis.
David Janes
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Thanks, David.

I think you are correct. If I'd ever paid attention I've forgotten it. I just pulled up a large-ish assembly, and it appears that Pro/E will use two processors for, at least, generating graphics / render mesh during the loading, changing shade quality, etc. Created an Envelope part with shrinkwrap feature of a complicated part and it only used one processor to create the feature, though. If I were to venture a guess it might use two for structural or dynamic analysis, etc.

Ok. Thanks, again.
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Thanks again David, Tried the processor_to_use. Comes up as a red circle in options. Pattern instance suppression works great, would never have thought to use the graphics area for that. Regarding learning the program, I've hesitated because, in part, the impression on the street is that a) Pro/E is the most capable modeler with the most features and b) partly because of it's multitude of features and partly because of a somewhat unwieldy UI, that it takes years to become even proficient much less a master of the program. After a week of study, I'm to the point where I think I can muddle through a design, at least one not too complex. I've even seen the logic to the pre WF UI. BF
wrote

less
config.pro
by your

processors,
design
single
without
broad, the

questions.
pattern
click on the

definition
SW!
the
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Autodesk propoganda, for the large part. At one time, when Acad was an up and coming thing, there was probably truth to it. Somewhere along the line, before my time (2000i or 2001? I started with WF.), things changed but the urban myth was already well established. With the introduction of WF & WF2 there's little truth left in it, though I can see where the most casual of 3D CAD users might still shy away from it.

I'm sure it does take quite some time to "master", even with formal training. There's a lot there.
- after about a year .... still a Fellow Newbie. Pro/E cuffs my ears regularly, but for the most part it's been a joy to use compared to what I was using.
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You're doin good, BF, and probably better, with a weeks' experience, than any of us in a similar situation would have done 5 years ago. It's getting easier and more user friendly. Many things still require some explantion but that's what this learning/teaching/helping community is about. Keep participating and you'll learn loads of good stuff.
David Janes
: Thanks again David, : Tried the processor_to_use. Comes up as a red circle in options. : Pattern instance suppression works great, would never have thought to use : the graphics area for that. : Regarding learning the program, I've hesitated because, in part, the : impression on the street is that a) Pro/E is the most capable modeler with : the most features and b) partly because of it's multitude of features and : partly because of a somewhat unwieldy UI, that it takes years to become even : proficient much less a master of the program. : After a week of study, I'm to the point where I think I can muddle through a : design, at least one not too complex. I've even seen the logic to the pre WF : UI. : BF : :
: wrote : > : Thanks David and J.Perry, : > : A much better and more detailed response than I had even hoped for much : less : > : expected. : > : With regard multi threading, I was referring to multiple processors : > : > Pro/e is capable of utilizing the power of multiple processors with a : config.pro : > option called PROCESSORS_TO_USE set to the number available and supported : by your : > operating system. Obviously, if your OS doesn't support multiple : processors, : > neither can Pro/e. : > : > : I will have to check out the Advanced-Draft option, since most of my : design : > : is in plastics. : > : The one thing that was not explained was how it is possible to make a : single : > : instance of a pattern independent? IE, suppress, delete or change : without : > : effecting the pattern as a whole. : > : > Sorry for the abreviated answer, but when questions are vague, general, : broad, the : > answers will be short and non-specific. Better answers require better : questions. : > So, have you actually tried WF2 patterning? Seems that, with both a fill : pattern : > and dimension driven pattern, it shows you instance positions. If you : click on the : > black dot, it skips regenerating these. If you want them back, you edit : definition : > and click them so they turn black again. Pretty simple, about as simple as : SW! : > : > : Thanks again, I think I'm actually starting to get some of it. : > : > Shouldn't take you that long since you're a newbie to Pro/e, but not to : the : > general concept, outlook and methodology of solids modelling. : > : > David Janes : > : > : : :
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Thanks for the encouraging words, and don't fear I'll be around as problems crop up. BF
wrote

much
supported
a
general,
fill
edit
simple as

to
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BF wrote:

Just out of curiosity ... what's all this above? Footnotes?
Regards,
--
#include <disclaimer.h>
Christopher Miller
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<<>> wrote:> Just out of curiosity ... what's all this above? Footnotes?
picky picky :-) You probably don't like top-posting, either.
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less
hyper
design
single
Hi BF,
You're welcome for the assistance. By the way, the Wildfire equivalent to the old Draft Offset functionality is called Edit - Offset. In Wildfire 1 and 2, you just set the selection filter to Geometry, pick the surface you want to extrude from, and then select Edit - Offset. From there, you select from the pulldown at the extreme left and choose the icon that looks like a tapered object. If you don't have an existing sketch to choose for your profile to extrude, choose References - Define and then you can re-select your sketching plane and horiz/vert ref plane for sketching. Then create your sketch profile. There's a cell in the dashboard area where you will be able to enter your draft/taper angle.
Best regards,
J. Perry
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without
select
a
be
Thanks again, Got it, though it seems to need a "starter" surface or solid. Easy enough to start with a feature smaller than the one I need. BF
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