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New user, seasoned CAD guy, with 3 curious quesitons

wogz

New member
Ok, so here’s my bit, a rant maybe. I’m an old Acad user, an AME user, a Mechanical Desktop user, and finally an Inventor guy. My new job has me in a Pro E environment, and I have been learning & using Pro E / Creo Elements Pro 5.. Some things I do like with Pro E, and there are some things I don’t. Like everyone else!! I do have a bunch of Acad habits, some hard to break, some easy. And of course, I do have the occasional wishes that Pro E performed like Inventor. But this is a CAD package, and like everything else, it has its own flavour. I’ve gone thru the Pro E university courses, and while they did get me up to speed, I do have a few reservations on that topic too. One thing is for sure, that Pro E resources & how-to’s are few & far between. This site seems to be one of the only extensive collection of help & advice. While I have found all I’m looking for, below are a few wishes and some questions I haven’t yet found answers to...

All or nothing. If I want to see a work plane, an axis, or a work point, you get them all, or none. No way (seems so) of turning on one or two, only one for a particular part or assembly. And the labels associated with.. clutter on clutter! In an assembly of more than 10 parts, that becomes [at least] 30 planes on at once! Any way to turn on one or two at a time?!

Parent / child dependencies.. Don’t get me started! Now, not only do I have to think about my design, but I have to think how I assemble the intended design just to see if it works.. A good hour or two wasted trying to get the assembly order right to drive a simple linkage to a rotating handle & shaft, which are both constrained to the same base part.. Inventor got rid of this since day one. Solidworks (form what I understand) also got rid of this concept.. It would be nice to slide the parts around while you constrain them too… Because, as per expected (an a law by Murphy) it’ll always snap to the wrong side, the wrong location as you assemble. Is there a way to move a part around in an assembly? to get it to the position you want without resorting to driving by constraints? or give it a constraint or two and then manually move to the intended position?

If I pick a surface to sketch on, why can’t it keep the view / orientation I’ve set it to.. It has to do its little dance to get the surface to what it want. I then move & rotate the view back to what I had, usually an iso view. That’s how I work. And why do I have to choose sketch references. Why can’t I just pick a side, and edge, a hole, a .. to reference my dims to?


So, anyone know if I can:

Turn on & off certain datum / work planes?
How can I move one part around in an assembly?
Can I stop it from 'dancing' when I want to sketch on a particular surface?

p
 
All three can be done without to much clicking. As for telling you how I could. At this time I choose not yo because I do not want to become an enabler . I have learned that everyone has to learn for themselves that way they learn things best and become self reliant.

I do advise you to review the Pro-e help files on layers & constraints for your first two questions. The third I think it would be best to check config.pro setting.

We have all been where you are now , best to enjoy the ride and keep an opened mind .

All the Best !
 
Despite what canoemike seems to think, we all learned FROM someone or something (no disrespect, Mike, I just disagree). It's late, so I won't give you as much detail as you'd probably hoped, but here you go:

Turn on & off certain datum / work planes?
- Set this up in your layer tree. You can add/remove datums from layers and then hide that layer. RMB on the layer and select "Layer Properties..."

How can I move one part around in an assembly?
- Ctrl-Alt-RMB and drag will move the part normal to your view
- Ctrl-Alt-MMB (middle mouse button?) and drag will rotate the part using its own center
- These will move relative to any relations you already have set, so keep that in mind.

Can I stop it from 'dancing' when I want to sketch on a particular surface?
- Not 100% sure I know what you're asking here, but I think the config.pro option you're looking for is:
- sketcher_starts_in_2d no
- And also you'll want:
- sketcher_refit_after_dim_modify no

Enjoy,
- Mark
 
regarding datum display, I have always found the method PTC employs to be pretty poor. yes, you can place different datums on different layers and then turn on/off those layers independently but then you're constantly moving datums to various layers when particular layers start to get cluttered or you decide you'd rather have one datum that is on one layer now on a different layer to improve clarity. or, you end up with multiple layers and you can't remember which layer has the datums you want to use and you start randomly hiding/unhiding different layers regularly just to find the ones that contain the datums you want to see/use.

I always found the way SW handled this far superior. you could turn all your datums off and never really need to turn them on. when you wanted to use a datum,
you could simply hover over the menu tree and each feature would highlight, including the datum in question. simply move up and down your tree and pick the proper datum as it highlights. easy. done. no questions. especially when you may have multiple datums coincident to one another such as in assembly mode.

Mark, i don't think the OP is asking how to move an individual component around in an assembly. I think he wants to have an assembly move based on mouse input such as a gear train or a yoke. For example, say you have a lever attached to a connecting rod which in turn attaches to a stopper valve (think toilet handle). in Pro E, you have to fully constrain the handle to the connecting rod and the connecting rod to the stopper. this is fine right up until you want to show what happens in the assembly when the lever is depressed and rotated through an angle of 20 degrees. in Pro, you have to change the assembly parameters to "move" the related parts and see how they work together. In SW, and i presume inventor, you assemble the parts how you want as they relate to one another but then while in assembly you can just drag the handle up and down and all associated parts connected to it will move accordingly. you can even set it up so that the components stop moving at an interference so if you have travel limiters built in you can simply adjust the handle from one stop to another and see how the linkage works.

but, I'm just guessing this is what the OP was referring too.
 
Mark seems to have answered your questions. I've learned a lot about layers and have made presentation on it that you might find helpful. Request it here.

On the parent child relationships, embrace this and they will become your ally. Think about your design and identify what the parent child relationships are. They aren't just a Proe / Creo thing, your design has them. That linkage won't work in the physical world if the parts aren't connected and sized properly. Think about how you can identify those and build them into your design models. Now those relationships in Proe are working for you, making your models work like the physical parts will. I've found that Proe shines and comes to life when you start building in ways that mimic how you might make them or assemble them in the shop.
 
Hi Guys,

Thanks for the replies.

Yes, what I was originally after was to move a part, an unconstrained part, or partially constrained to a desired location “If I put my bracket there, what do I need to change? Do I need to modify another part? Is the bracket long enough to reach?” . (Remember, I’m an old Inventor guy, you could move parts around as you wished. Just click and drag) And yes, I did find it. CTRL & ALT and the RMB.

But as Mike pointed out, there are more to constraints then expected. I’ve had a crash course this morning with Pin & Cylinder constraints. Way cool (but overly cumbersome for the intended purpose. But I get it.) So, many ‘insert’ constraints have changed to ‘pin’ constraints. And I’ve set the limits too (that took a bit of thinking to get right!) And yes, Michealpaul got it right. Inventor you can try the linkage movement right from the first constraint added (actually, you can constrain a sketch and have it act as you want, without all the modelling if you so desire.)

Again, with Inventor, you can see the work planes, in the tree, turn on what you want, turn off what you don’t. Parts come with their base planes, and you add as you want. One issue I think I’ve run into, is the bad habits of my co-workers. They don’t use the work planes (or layer), so they are all on the one layer (or on the default layers), or they leave them all on, or.. Whatever the case, I will look at the layers & layer plane controls. I just need to sit & decipher what they (layer) all are in my assembly; which do what, associated with what part, and so on..

And yes, will look into the config.pro later. I’m under the impression that our config.pro affects each user in the department, so we all need to ‘buy into it’. Will look at that later too.

Next question.. Is there a way to turn on the dimensional references? Like, the first dimension I put doing is D0, then D1 for the next, and so on. In Mech desktop & Inventor, you see the dim designator, so it's easy to say D15=d4 or d65=(d2/2)+d6 or the like, to get true & fast parametrics. I'm given the impression that in Pro E, you need to set up 'relations' as you build, and create 'parameters' for certain numbers you intend to use.. rather than just grabbing them on the fly. I know I can make an equation in the dim field, but haven't found their designators..

p
 
You can use the 'switch symbols' command to flip between dim symbols and values. I don't recall where it is in CEP 5. If you enter the relations dialog (tools -> relations) it'll automatically switch to the symbols.

You can load multiple config.pro files, one for the company and one for you. They load consecutively, starting with the 'text' folder of the installation, then the user's 'home' directory (as defined by Windows) and then the directory defined in the 'start in' field for the icon used to launch Proe. They are additive, meaning one file adds to the next, unless an individual option conflicts. In that case the later file overrides the earlier one for that option only. The exception to that is the config.sup file which must be in the text folder. Options in it can no be overridden by later files. You can also load files manually through tools -> options.

oh, and check out ptcuser.org and the community forums at ptc.com for more help
 
Despite what canoemike seems to think, we all learned FROM someone or something (no disrespect, Mike, I just disagree). It's late, so I won't give you as much detail as you'd probably hoped, but here you go:
Enjoy,
- Mark

"no disrespect, Mike " None taken. Yes, I am sure I sounded heavy handed. All I am pointing out is to show initiative and become aware of resources instead of reaching out every time there is an issue. I have experienced it many a times , instead of trying it three times a user will just keep asking questions of someone else. I am sure I will take some heat but I would prefer not to "catch the fish for you" .

Good luck Wogz on your Pro-e Journey !
 
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thanks again all...

Thanks Canoemike, I like a good poke! haha!!

Just trying to figure out all the little fiddly bits!
 
there are some things PTC programmers could take from autocad of 30 years ago to make basic improvements with layers etc. sounds like your making improvements.
 
OK, found how to display the dimension parameters as a variable, a designator, not just numbers.

Next "hurdle" is how to use them.. properly I guess (didn't think this would be soo hard!!) I've made a relation, d12=d3-.125. great, I get a number. Oops, I should have called up d4, OK, double click to change.. double click to change.. click edit to change.. check the relations table to change.. OK, pick the value to change... Uhm what do I click to get this relation to show, so I can edit a variable?

(The other CAD program I've used, I can click the value, it'll show me the formula in the dimension box, and I can change what I want right there.. Pro E has it hidden somewhere..)

anyone?!
 
Tools -> relations

One thing you might want to do inside the relations dialog is comment your relations so later you remember what they do. Adding /* in front of a line makes it a comment.

Also, note there are two areas for relations, initial an post regeneration. You toggle between them using the drop down in the lower right. Initial relations are evaluated prior to regeneration, post regeneration are evaluated after. Most of the time you want to use Initial (and if you type an equation in for a dim that's where they end up). Relations that drive parameters reporting mass properties, for example, should go in post regeneration so they'll reflect the updated geometry.
 
OK, found it..

(thanks dgs!!)

Found it, it's under relations, which is where I thought it might be. But it's actually a relation related to a feature, so you have to go into relations, then select feature, then select the actual feature. then you get it..
 

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