What is WF 3 asking of me?

[cityjack]

Alrighty,

I am confused a tad here. I make a datum plane on the fly as my sketching plane. I accept what pro gives me as a normal plane to my sketching plane to orient the sketching plane normal to the screen. Same as the last twenty years. It pops up a dialog box saying you do not have enough references do you want to sketch anyway? I say yes and away I go. What is it having trouble with and why is it asking me for more references? Also sometimes when I think I have selected my two planes, a sketching and an orientation plane, at the end once I want to exit sketcher it tells me I don't have enough refereces to place the sketch and will not let me get to the extrusion or cut part. What else do I need? I gave it two planes, dimensioned it. I am confused. Any help would be greatly appreciated. Good morning by the way.

Sid

 

[[-Skint-]]

It sux sometimes doesnt it

A horizontal reference and a verticle reference usually will suffice.

 

[Mindripper]

I guess some sort of third reference is required: a vertical plane/surface/edge, or an axis/point. But (as you noted) this doesn't have to be defined prior to starting to sketch. Just make sure one of your dimensions or sketch points is explicitlyconstrained to a feature that provides a reference clearly tied to asecond direction in the sketch plane.


Are you new to Wildfire? There are some added 'features' in the sketcher, esp. the 'Strong' and 'Locked' dimensions.

 

[cityjack]

Yes I am ABSOLUTELY new to Wildfire. I went from 2001 straight to WF 3. My last company didn't want to continue to pay the maint. fee so I was left at 2001 while everyone else was forced to use Solidworks. Now my new place of employment is at WF 3. Alot of things have changed. I haven't EVEN ventured into the drawing aspect yet. Just as always I guess, since version 2.5 on a Sun Sparc 1 Unix station, I'll adapt. thansk all for your help.

Sid

 

[Mindripper]

Do you have access to PTC University? I used Pro/E release 17 thru 21 from 1997 to 2001, then got to experience the pleasure of running SolidWorks until last March: I love SW. Now I am back on Pro/E, and WF was brand new to me. I work for a great big company now, and have full access to the training 'tapes' on PTCU. I took the 'Fast Track' courses and a bunch of others, mostly as refresher courses. These are actually quite useful, but I don't think they ever mentioned 'locked' dimensions.


Locking dimensions is handy for dimensions you don't want to vary as you alter the sketch; they are just a right-click away. They aren't actually locked: you can still edit them.


Not much has changed (read that improved) on drawings in Pro/E since 2001, unfortunately. It's a real downer for me, after using SW's great (and continuously improving) drawing package for five years.

 

[mjcole_ptc]

The following are new sketcher config options in WF3. I believe you may have the following config option set in your or your company's config.pro file. I've explained this and other options below.

sketcher_auto_create_refs 0
This would prevent Pro/E from auto selecting 2 references usually default datums as references. You can fully constrain any sketch with the default CSYS as a single reference. Also for sketches where you are only going to use the Use Edge option dimensioning references are not required.

sketcher_palette_path X:\Path\to\Sketcher_Palette_Folders
Allows you to add a folder containing named folders with .sec sketches. These folders become tabs in the Sketcher Palette tool.
sketcher_undo_reorient_view yes/no
Self explanatory
sketcher_auto_create_refs 2*,1,0
This option allows you to prevent Pro/E from picking Right Top or Front as the two section references.
2 Is the Pro/E default and I have always found it annoying.
1 Automatically adds the Orientation reference as the first ref and allows you to choose the second.
0 Lets you choose the references you want.

sketcher_dimension_autolock no*,yes
This option differs from sketcher_lock_modified_dims because it locks dimensions when you create them or make them strong without having to modify the value

Michael

 

[super_puh]

I think the only reason that any one works with PRO/E is that there are companys that started with PRO/E along time ago and all of theirs documentation is on PRO/E and they do not have any choice but to continue with PRO/E.


To bad thats are alwaysbig companyslike the one I work for.


I love SOLIDWORKS too

 

[Mindripper]

Oh God, the endless config.pro options. Can't we just make models without the need to learn the royal hieroglyphics? But sketcher_auto_create_refs 1 appears to be your solution, cityjack. And thanks mjcole_ptc; I will add these to thegrowing list of config.pro options in my Pro/E notebook.


Curiously, I don't even have an SW notebook: don't need one. Never did.

 

[robrific]

Alrighty,
Also sometimes when I think I have selected my two planes, a sketching and an orientation plane, at the end once I want to exit sketcher it tells me I don't have enough refereces to place the sketch and will not let me get to the extrusion or cut part. What else do I need?


Sid

Are you holding Ctrl before you select the second plane?

 

[tosh382]

City Jack !

Use the Advanced User sketcher ... which is easily found by turning off the intent manager.


Add/remove dimensions or add/remove contraints or add/remove alignments by the way you think and now how the fuzzy logic thinks ...


Of course if you have to use the regenerate menu selection manually ... and you must be zoomed up tight so things don't align with other things ... if they are only .020 apart from each other ... zoom to make them look like they are .500 apart, then regenerate and get out of the sketch.


===========


Another matter using the Intent manager is: "Don't put somuch stuff in the sketch .. you can add many features to the tree today ... as there are CISCIntel processors inside and not RISCinside ! <SMILE>
Edited by: tosh382

 

[jelston]

I think the only reason that any one works with PRO/E is that there are companys that started with PRO/E along time ago and all of theirs documentation is on PRO/E and they do not have any choice but to continue with PRO/E.


To bad thats are alwaysbig companyslike the one I work for.


I love SOLIDWORKS too

Amen. I don't think the biggest problem I face in a day should be the design software that I use

. And yes, I love SW too.
Edited by: jelston

 

[mikewal]

Mindripper, I too worked with Pro 17 -21, moved over to SW for years, changed jobs and was dumped back into WF. I completely agree with you. Sw is definately the better package.

 

[cityjack]

Thank you all for your help. I see how turning the intent manager off gets me basically back to pre-wildfire. No I was not holding down the Cntrl-key when I selected the second plane. Didn't know I had to. I will see if I can get to the PTC university thing. I know I have an account. Just gotta look around for the classes I guess. My new boss here wants me to enroll for the Elearn thingy from PTC. Not too sure if that'll do me any good. It seems 9 times out of 10 I do anything with help through ptc it always tells me what I already know or doesn't tell me anything I want to know. I'd like the option of actually asking something I'd like to do. Not always follow a "DUMB" sylabus. A human is nice every now and then. I cannot see making this company pay for something that will not help me. Going to look for the classes now. Oh, and thank you for the config.pro help too. This sight is the sh*t! I feel like I need to set up an automatic debit to you guys.Almost. I'm out. Have a good day all.

Sid

 

[cityjack]

I have put the config.pro option of sketcher auto create refs in and still it takes references it wants automatically and still wants a third orientation ref. My config.pro is in the text folder and all my other options are working fine. Option set to zero as well. Is there something I am not seeing here?

Sid

 

[cityjack]

Oh yeah 1 more thing. I lied. there is another option that is not working either. I entered feature_create_auto_begin in as well. It is set to yes to prevent from having to pick define all the time. It as well is not working. Thanks.

Sid

 

[cityjack]

Seems I have answered my own questions. Just to forward on the info in case anyone ever encounters the same thing. Or maybe I am the only knucklehead that didn't have a clue. Anyway, the feature_create_auto_begin setting set on yes only works for non-dashboard ONLY features. And the sketcher_auto_create_refs set to 2 just gets rid of the extra ref dialog. It doesn't keep pro from picking the second ref in the original sketcher setup dialog. If that makes any sense. Thanks for your help though.

Sid