Collision in Wildfire?

I cannot figure out how to simply move a part in Wildfire and test for
such things as detecting collision. Can anyone point me in the right
direction? Do I need to use Pro/Mechanica?
Reply to
SR
Loading thread data ...
: I cannot figure out how to simply move a part in Wildfire and test for : such things as detecting collision. Can anyone point me in the right : direction? Do I need to use Pro/Mechanica?
Motion is handled somewhat differently than in SolidWorks. Parts are assembled with 'connections', a way of defining degrees of freedom between two parts and making them moveable. Then they are moved to Mechanism Design where they are 'motorized', given a motion definition and then run through studies, testing both the motion defintion and the assembly. A feature of the study of the assembly in motion can be checking dynamically for interference throughout the assembly. Mechanica is not needed for this particular function.
David Janes
Reply to
David Janes
David,
Since you guessed I have experience with SolidWorks (actually my company is currently evaluating these products), I wonder if you can help me to understand a couple of other differences I'm struggling with? I'm using this ng for two reasons - to keep the reseller sales reps away as well as see what the product ngs are like. I hope I don't start a fury of negative input from others, but I'm sure I'm not the only one out there that is looking at replacing their CAD system. Please DO NOT take my questions below as a sign that I am favoring one product over another; it's just that I began my evaluation with mid-range products. I'm pretty good with part modeling now and am currently reviewing the assembly design tools:
1. SW has what they call lightweight parts where you can gain performance opening and working with large assemblies. They have an option to open lightweight as well as switch between lightweight and resolved states. I have not been able to figure out the equivalent in WF. The closest thing I have found is geometry reps vs. graphics reps? Can you clarify for me what the equivalent is in WF and where I get more info on it?
2. While in an assembly file, I can't seem to find anyway to select multiple parts quickly such as using a 2D or 3D fence? SW uses an envelope (actually kind of awkward if you ask me). How can you select more than one part to hide them?
3. SW has some tools to locate parts in an assembly like "Zoom to Selection" which zooms in on a part in the graphics window and "Go To Part" which locates the part in a complex assembly tree. Is there any equivalent in WF?
4. I find as I learn WF, the interface keeps switching from an icon-based (toolbar) approach to the Menu Manager. Is this a hold-out from Pro/E or do you know if WF will eventually replace MM with more toolbars?
TIA, SR
Reply to
SR
Steve, this post of yours was addressed to David, but I figured you can use a second (and third) opinion as well. I mostly use Pro/E, Release 2001 until very recently, and have just completed my first small project in Wildfire. I also use SolidWorks quite frequently, although I try to avoid it unless my customers insist on it. I have not yet used the latest release, SolidWorks 2004, and am being told that it is much better than SW 2003. Please bear in mind that all I am going to say relates to my experience with SW 2003. If you search this NG, you will find many threads discussing a SW vs. Pro/E topic. I have posted some detailed (oftentimes probably too detailed) rants about stuff I dislike in SW in some of these threads. Here are my answers to your questions:
The Pro/E analog is called 'simplified representation'. It is only available in the Advanced Assembly module. So nominally 'basic' SW is ahead here. However, here is my experience: I have worked with Pro/E assemblies of nearly 1,000 parts without any simplified representations and very seldom have had to wait for my PC. On the other hand, SolidWorks assemblies with less than 100 parts are often becoming quite slow to handle. So, IMO, SolidWorks had to throw in the lightweight parts just to allow their program to be marginally speed-competitive with 'basic' Pro/E. The fact that SolidWorks part files are much larger (often 2-3 times) than Pro/E parts, and that SolidWorks assembly files seem to be roughly equivalent in size to the sum of constituting part file sizes, which makes them sometimes 20-50 times larger than the same assembly file in Pro/E, doesn't help SW at all.
If I am not mistaken, there are 2 or 3 different fence-type selection tools in Wildfire. However, I have not tried them yet, because I have developed a habit of selecting multiple parts in the assembly tree, rather than in the graphics window. By the way, I do it the same way in SW as well. I believe it is a more reliable way of multiple selection than using the graphics window, anyway. The selection toolbar is not being shown by the default installation of Wildfire. You'll need to customize your toolbars to show it.
I am not sure about the 'Zoom to selection' in Pro/E because I've never tried to find it. In Wildfire, if you put your cursor right on the part you want to zoom on and start rolling the mouse wheel, the zoom in function will automatically recenter your window on this part anyway. Again, both in SW and Pro/E I try to use tools that allow me to do what I want without leaving graphics window, rather than go and click one more button. As far as 'Go To Part': when you click on the part on screen, Pro/E will highlight the part name in the tree. However, there is, as far as I know, no way to roll the tree display to show the part or expand the subassembly to show the part belonging to it, the way SW's 'Go To Part' does.
Yes to both: the text menus are the remains of the previous Pro/E GUI, and yes, they are going away. I have heard that in the next release, Wildfire II, there still are quite a few, so the earliest when all (or nearly all) text menus are replaced by buttons will be Wildfire III.
Reply to
Alex Sh.
: I hope I don't start a fury of negative input from others, but I'm sure I'm not the : only one out there that is looking at replacing their CAD system. : Please DO NOT take my questions below as a sign that I am favoring one : product over another; it's just that I began my evaluation with : mid-range products.
No apologies needed, no criticism warranted. And, none forthcoming, it seems, so you can relax. Lots of the people in this NG, as Alex indicated, have used other CAD packages. Some go back beyond the 2D dinasaurs of CAD to actual board drafting (art with a straight edge and dividers, the alleged legitors of Da Vinci.) That may be the only dividing line that gets people excited ~ drafting (glad it's dead or dying) and solids modelling. That statement alone could cause more romantic outcry than anything you've asked, so far. But you won't find much partisanship, here. We're users of Pro/e, not salesmen. As you'll find in the SolidWorks NG, since we know the software the best, we are also its best critics. We know its strengths and weaknesses. We have no interest in hiding anything. So, you've made a good decision to come here. Feel free to fire away.
: I'm pretty good with part modeling now and am : currently reviewing the assembly design tools: : : 1. SW has what they call lightweight parts where you can gain : performance opening and working with large assemblies. They have an : option to open lightweight as well as switch between lightweight and : resolved states. I have not been able to figure out the equivalent in : WF. The closest thing I have found is geometry reps vs. graphics reps? : Can you clarify for me what the equivalent is in WF and where I get : more info on it? : I would only add to what Shishkin has said by pointing out the forest. When you look at Pro/e, it is sometimes hard to tell the forest from the trees. It's huge, and even if we were to continue on the issue of assemblies and the Pro/e equivalent of SW 'collision detection', we'd have to go into three separate modules of Pro/e. But, in the process, we'd find out that SW has nothing to match, nothing even close to what Pro/e's Mechanism Design has ~ not even in the same ball park. But, it's quite enough for many people who don't need the sophistication and complexity of Pro/e.
Further on this point of assemblies is the fact that Pro/e has a whole philosophy and varied technology of top down modelling. Simplified reps are one aspect of it. So are skeleton parts, interchange assemblies, shrinkwrap models, family tables and half a dozen more model and assembly functions and processes to accomplish what the one 'lightweight' model in SW accomplishes, i.e., help manage and speed up the use of large assemblies. It's really difficult to compare with SW, the whole program could be considered 'lightweight'. Makes you wish to see something like a Consumer Reports feature/price/value analysis of major software packages. So far, they all seem kind of shy to submit themselves to anything like that, preferring instead to have 'design wars': 'our users make big, complicated stuff instantly with our software, bigger and faster than the competitors' brand'. Well, I worked at Motorola and Caterpillar which each depended heavily on Pro/e. But, in each case, many suppliers and vendors got dragged along for no conceivable reason except that these two giants demanded it. So, it much depends on your industry, your suppliers, vendors and competitors, and probably lastly, whatever software you can get away with investing in, that determines a software purchase decision.
David Janes
Reply to
David Janes
...
This is incorrect, simplified reps have been part of Foundation Advantage for a year now.
...
Reply to
TH
Thank you
Sorry for the one word replies, but "Agreed"
I actually think the lightweight part technology is pretty good (that is the ability to open large assemblies with or without the feature data). I think there is some value in it. By opening an assembly lightweight they are just loading the graphic data into memory thereby increasing the speed on open. I did some timing tests on a 3000 part assembly and found the lightweight vs. resolved (non-lightweight) helped significantly. Not to sound pro-SolidWorks here, I also found some limitations. Overall, I like the fact that it's automatic, no setup, no suppressing features or converting data it's just there as an option. I have not been able to test an equivalent assembly in Wildfire, but so far I have found the small assemblies I have built and the ones I have seen in demos to be pretty slow on load and response time.
You're going to think I got sucked to their brainwashing, but I really don't see anything wrong with this. At the end of the day it's all about productivity. I have heard people tell me that ProE has a 6 month learning curve and after 1 month, I'm starting to believe it. I was creating parts in SolidWorks and Solid Edge (the other product we're looking at) within the days while I still find I'm lost in Wildfire! I'm getting better though and see more that I like...
Well,
That's why we're putting the effort in. The fact is, we're investing in a solution for the long term. Thanks for you feedback.
Reply to
SR
I'm not seeing the differences in speed you're seeing, but I agree with the file sizes.
Thanks, but I haven't any fence tools for selection. As for selecting from the assembly tree instead of graphics, I was really hoping there would be more tools here. I could see if the assembly was 100-1000 parts, but most of our machines are 3000+ with some exceeding 10000 parts. Having to select parts from the tree could be very time-consuming. Does Wildfire have anything that compares to the SolidWorks envelope?
Thanks
Thanks, I read the list of changes expected for Wildfire 2.0.
Reply to
SR
: > : : I actually think the lightweight part technology is pretty good (that : is the ability to open large assemblies with or without the feature : data). I think there is some value in it. By opening an assembly : lightweight they are just loading the graphic data into memory thereby : increasing the speed on open. I did some timing tests on a 3000 part : assembly and found the lightweight vs. resolved (non-lightweight) : helped significantly. Not to sound pro-SolidWorks here, I also found : some limitations. Overall, I like the fact that it's automatic, no : setup, no suppressing features or converting data it's just there as : an option. I have not been able to test an equivalent assembly in : Wildfire, but so far I have found the small assemblies I have built : and the ones I have seen in demos to be pretty slow on load and : response time. : Well, isn't one of the 'limitations' that, once open, there's not much you can do with it? Can you use it for assembly modelling? That's a huge plus in Pro/e, however long it takes to open. Can you swap parts in and out? Can you speed up part creation and part substitution with family tables, interchange assemblies, layouts, skeleton parts and assembly relations? Who cares if it loads fast but you can't do anything with it!?! Pro/e doesn't entertain a 'look, don't touch' approach modelling and assembly, although, high levels of protection are possible.
: > So far, they all seem kind of shy to submit themselves to anything like that, : > preferring instead to have 'design wars': 'our users make big, complicated stuff : > instantly with our software, bigger and faster than the competitors' brand'. : : You're going to think I got sucked to their brainwashing, but I really : don't see anything wrong with this. At the end of the day it's all : about productivity. I have heard people tell me that ProE has a 6 : month learning curve and after 1 month, I'm starting to believe it. I : was creating parts in SolidWorks and Solid Edge (the other product : we're looking at) within the days while I still find I'm lost in : Wildfire! I'm getting better though and see more that I like...
In a couple hours, I could get the average modeller of either package, doing flat plates with holes, on the other package. Depends on what you need to do. The more complicated it is, the longer it will take, on either package. And Pro/e will do more complicated things, period. No???? Okay, what's SW's solution to creating a bolt in increments of a quarter inch? Copy/modify? When is SW going to get table driven families of parts, created by 'instantiating' a generic with the click of a button ~ pick a dimension (or two or more dimensions to vary by, plus increments), then just go back and give each instance the name of a part in stock. Include parameters, descriptions, vendors, manufacturers, price, material, unit of measure. You could create multi-level families ~ metric on one side, u.s. customary on the other, then branching by thread pitch or socket size or any other criteria deemed useful. Productivity features abound in Pro/e. But, what I've learned about the software is this: it's heavy on the front end, going in ~ heavy investment in money to buy, heavy investment to learn (each new productivity feature, like family tables, takes time), heavy investment in getting the system set up and functioning to the satisfaction of most (never all). But, once the productivity features are in place, they begin to pay dividends. It's just that, for the impatient, the time frame may be a bit too extended.
Hope you have the patience and a long enough view.
David Janes
Reply to
David Janes
FYI, SolidWorks DOES have family table functionality, but they call it configurations.
Pretty much the exact same concept as Family Tables in ProE. But, IMO, Solidworks' configurations are a little more flexible (better) than ProE's Family Tables.
Reply to
Arlin
The issue of configuration tables was 'touted' to be able to use MS Excel in version PRo-E v200i^2, or was it 2000i?
SURPRISE, the implementation was awful and did not work as expected. It still doesn't work well enough to use daily in Wildfire, and not nearly as well as SW has since 1996.
Pro-E vs Solidworks / Edge / etc... has been hashed before, but for my uses in die making the following is important to me and ignored by PTC.
HUSK HEALING
A major feature in the solid model kernal that seems to be missing in pro-e vs parasolids-based modelers. Is this why I get 'cannot intersect feature with part' error messages in Pro-E ?
ACCURACY
I NEVER had to set/reset/coordinate the accuracy between the parts I was merging/cutting out in SW. This is a constant issue in Pro-E. Also, features in PRO-E can be created that have hidden 'GEOMETRY CHECKS'. Necessitating continual checks of the model integrity during design.
'SLIVER FEATURES'
See above. Is this why I get 'Cannot intersect feature with part' error messages in Pro-E?
UNITS
Pro-E does not recognize units for feature entry. Sure you can change the units globally, but you cannot enter the following dim: 1.00"+5mm
Minor gripe, sure. But with the local shop working in inches, and more and more standard hardware designed in mm, entering 40mm in sketcher or family tables is less confusing and better captures 'design intent' than entering 1.575
There are also intances where Wildfire was not thought out well. For example, in drawing mode the 'new colors' makes hidden lines almost invisible relative to the default background color. Overall the entire color scheme change for feaures in Wildfire makes one wonder. Why change surfaces from purple with yellow edges to blue-violet with red-violet edges (very hard to see). Why change planes from Red and Yellow to Brown and Black (also hard to see). I can't believe that someone at PTC saw this and though that it was 'good enough' to ship.
Now for the Good news...
Pro-E Wildfire (v24) seems to be more robust in the following areas:
ROUNDS / FILLETS
Better, but still fail whend dealing with rounding over draft, or rounding into profiles that are not 'straight'
DRAFT
Completely redone. Seems more robust. Existing parts with draft when modified bring up old draft menus. New draft must be using new code?
THICKEN
More robust than surface/offset. Will swallow surface patches.
Still needed...
see above and the following:
Allow for non-uniform scaling as a feature in the feature tree in the base foundation package.
Put back 'Insert/shared data/Copy Geometry from other model' into the base foundation package.
Reply to
Chris Gosnell
Actually, you can pretty much do anything with lightweight parts in SWX. SWX just automatically loads the lightweight parts when it needs to access the full dataset.
This has the effect of loading very quickly, but while working on a model, there can be pauses when SWX has to go out and fully load a component that was originally lightweight.
Thus, it is a tradeoff. Some prefer not to use lightweight and load everything up front to prevent the pauses that can happen later. Often, these people work with smaller assemblies and/or they are working with/modifying most of the components during their session.
Others prefer the usage of lightweight parts. These people often are working with some very large assemblies and/or they are not making very sweeping changes that modify most of the parts, thus requiring the parts to be loaded.
I am not trying to start or continue a ProE vs SWX flame ware here. I just want everyone to know the facts.
Reply to
Arlin
I'm not a SW expert, but the real advantage I see with this technology is memory consumption. The larger the assembly, the more control you have over your resources. As I mentioned, the nice thing about them is that it's automatic meaning you don't have any setup to take advantage of it; you simply decide whether you want to work with reduced memory requirements or all geeometric data. If you're working in lightweight and need all geometric data (i.e. for interference, motion, etc.), you simply toggle the part to 'resolved'. I believe simpilfied reps are also a method to control this as well as other capabilities I'm discovering. I keep asking this question because I have read how Wildfire includes "lightweight components" , but just couldn't find out how to compare them when finally I found out what they were talking about. There is a new simplified rep type called "lightweight" with Wildfire. I don't see this as the decision breaker, but I also don't think it should be taken lightly.
I appreciate your feedback. The final decision will be made Feb 27th so that gives us another 6 weeks to complete our research and submit our results. Hopefully that's enough time.
Reply to
SR

Site Timeline

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.