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Over constrained section?

B

bhayden

New member
I don't understand why this section needs all four of these dimensions: 1.660, 1.500, .080, 45 degrees. It seems like any three of the four completely constrain the section. Note that the section is also constrained to be symetric about the centerline. (sorry about the rotation)



View attachment 54
 
No, it doesn't need all those dimensions. In fact, to save on all the sketching, only one side of the feature needs to be sketched, then you could mirror about the center line
 
I agree that it shouldn't need all of the dimesions but if I delete one it adds another weak dimension somewhere else. For some reason Pro is convinced that it needs this seemingly redundant information.



To make matters worse when I tried to exit sketcher (having given up on removing the redundant dimesions) it failed with the message that the sketch must be a closed section. I went round and round trying to figure out why it didn't think this was a closed section. Finally I saved the sketch as a .sec file. I then started a new part and used the insert data from file option to bring in my saved section. Low and behold it had no problem with it being an open section. This is the second time in a couple of days I've been burned by this behavior. Anybody else seeing the bogus not a closed section thing.



-Bernie-
 
I recreated the sketch from your picture. I created half of the sketch and then mirrored it. I used the required or needed dimensions. It did add an extra wick dimension. Then I went back to Sketcher (pulldown) and unchecked the Intent Manager. I regenerated the sketch with the extra dimension and it did ok. Finally I DELETED the extra dimension and regenerated the sketch. It did ok and Done. I hope this helps you out.

AS
 
My guess would be that one of the intersections was not properly joined and connected, hence the open section warning and extra dimension. It needed the extra dimension to define the endpoint of one of the lines.
 
especial,

If I understand correctly you were able to get the exact same section to regen both with and without the extra dimension when intent manager was turned off?



lcoates68,

I too thought that perhaps the section wasn't properly joined and that was causeing the open section warning. However, according to analysis the distance between the end points was zero. I deleted and redrew the lines; same thing. The real kicker is that when I saved the section and then brought it back into a new part using Insert > Data from File it worked just fine.



I can only conclude that this is a nasty BUG in Sketcher that I've bumped into on several occasions and wasted a ton of time thinking I was doing something wrong.



I'm still working in 2001, I'd be interested to know if this is fixed in WF.



Bernie Hayden

XKL LLC
 
Bernie,



Please upload this file into the forum. I'd love to see this for my own eyes. Trying to recreate this from your sketch will not solve anything. If there is some sort of bug, I don't think I'll be able to recreate it. If you upload the sketch, I think I can figure out what is wrong.



Later,

Greg
 
Yep If for some reason the sketch is telling you something is open do a Trim Corner. I do check of the Intent Manager about 25 percent of the time.

AS
 
In cases like this, I typically dynamically modify a suspect dimension with the dials in the Modify dialog box and see what happens. This usually points out my problem, which 90% of the time something is not constrained properly. Would like to download the sketch though!
 
I do the exact same thing that Jason said when I run into situations like this. Many times modifing the extra dimension will cause an unconstrained endpoint to move and identify where the problem is.
 
Okee Doky,



Here goes trying to attach a file to a post. If all works correctly anyone interested should be able to download examples of the sketch in question.



-Bernie-
 
Thanks to all who reminded me that the best way to investigate a nonbehaving section is to modify one of the dimensions and see what moves that shouldn't.



Thanks to Greg and Jason I think we've pinned down the problem to my use of the default trim option Dynamically trim section entities. If instead you use the second option on the fly-out Trim entities (cut or extend) to other entities or geometry. the endpoints of the trimmed lines are left attached.



IMHO the first trim option should be fixed or eliminated. It's a prime example of little land mines PTC leaves scattered about their products (like lower case entry only in Intralink, thank you very much).



In conclusion, as Greg said:

I think we have this figured out, God bless the forum.



AMEN to that brother!!



Bernie Hayden

XKL LLC
 
You don't have a problem (BUG). It took me 15 second to find the problem and fixed it. Now how much time did you spend on it? I did it per what I mension above.

AS



Alway think how you can beat Proe .
 
To be more specific you do have an open sketch. The horizontal line (0.6710) and short angle line Do Not Touch (two corner). Zoom, Zoom, Zoom, ... that corner and you'll see they don't touch.

AS
 
Not a bug? You're given two tools to trim lines and one (the default) produces an erroneous result. I'd call that a bug. Having a section that generates an error as drawn but imports without a hitch, I'd call that a bug.



Seems like those in the know avoid at all costs the Dynamically trim section entities tool. Knowing how to resolve issues with workarounds is all too common a reality with ProE and I believe a contributing factor to it's reputation of being hard to learn and use. I'm curious, does WF react the same way (bug compatible)?



The answer to how much time I've spent; a good hour or more on this part writing up the problem and responding to the forum. Over the course of the last couple years the amount of time lost to believing that the Dynamically trim section entities worked correctly; many many hours. Several times I've fallen back on creating geometry in Cadkey to import because of this issue of coincident points not being recognized as such and the lack of tools in sketcher to analysis the problem.



Alway think how you can beat Proe .



What is this supposed to be, a video game or a mature, best in class CAD system?



-Bernie-
 
More foo,



If you're trying to recreate this bug I've found that an essential element of the failure is that the top of the rectangular section is coincident with the horizontal reference (the graphics in the original post are rotated 90 degrees). If the top of the section is not coincident with the horizontal reference both Dynamic Trim and Trim to other entities seem to work just fine.



I believe that if you draw just a simple rectangular section and the 45 degree notch you'll fine that you can create a section with Dynamic Trim that appears closed no matter how far you zoom in but still fails with the not a closed section error.



-Bernie-
 
Bottom line I'd call that a bug, So it is a Bug, I'll go with that.



Always think how you can beat Proe

To me, I see it as a challege, to others it could be frustration.



I apoligize for not seeing workarounds as a Bug.



AS
 
Does anyone use the default Dynamic Trim? I have never been able to figure a use for it. Too bad you can't replace it in the menu with the always used trim?
 
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