Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Dimensions randomly scatter

I

iland99

New member
Ever since switching to Wildfire we have had a problem with dimensions randomly scattering across the drawing. It will scatter the dimensions after regenerating the model, switching sheets on the drawing, or updating views. There is no pattern as to when it will do this. You can regenerate the model or drawing 12 times with no problems, and on the 13th time it will scatter the dimensions. PTC suggested that we set the config option "associative_dimensioning" to a value of "yes". This seemed to reduce but not eliminate the problem. We were assured that this problem would be taken care of in 2.0.


Now that we have switched to 2.0, it seems like the problem has gotten worse. Even the config option doesn't seem to be helping as much as it did in Wildfire. This is an EXTREMELY frustrating problem, as you could imagine.
smiley35.gif
It'sgotten so badthat I save every sixty seconds or so. That way when the dimensions scatter everywhere, all I have to do is erase the drawing from memory and pull it back up, rather than spending 10 minutes moving the dimensions back to their original positions.


Has anybody out there experienced anything similar to this? If so, were you able to fix this problem? Is there a better way of dealing with this problem?
 
I have never had the problem. Do you use snap lines in your drawing to control their spacing? They might help.
 
dr_gallup said:
Do you use snap lines in your drawing to control their spacing? They might help.
Click to expand...


We don't use snap lines very often, but I started using them after this problem started happening to speed up the process of getting the dimensions back to where they should be. It doesn't seem to make a difference one way or the other. They scatter regardless of whether snap lines are used or not.
 
iland99 said:
dr_gallup said:
Do you use snap lines in your drawing to control their spacing? They might help.
Click to expand...


We don't use snap lines very often, but I started using them after this problem started happening to speed up the process of getting the dimensions back to where they should be. It doesn't seem to make a difference one way or the other. They scatter regardless of whether snap lines are used or not.
Click to expand...
 
I have had the same problem and have not yet found a solution yet. It does not matter if you use the snap lines or not, the problem still occurs and I am on the latest version of WildFire 2.0.
 
We also have some drawings of complicated geometry whose dimensionsdisplace at random. We have not found a solution to the problem.
 
Hi Everyone,


Me to. I have faced it lot many times in WF 2.0. If there is any Soln. please let me know.


That makes horrible in assy. drws.


With regards,


Mani
 
Me too !


Have you guys found the views get thrown around when this happens also ?


If anybody has a solution to this very irritating problem then I would be a happy man.
 
MartinBooker said:
Me too !


Have you guys found the views get thrown around when this happens also ?


If anybody has a solution to this very irritating problem then I would be a happy man.
Click to expand...


Hi,


I accept with Ur Point but U can control Views from getting thrown.


The problem may occur when U resume UR suppressed features/parts, because Proe will place the views in drawing based on its centrepoint. When U resume the components/features it may grow more from the actual size of the model.


Solution:


When u place a view in DRW just go for prop & there will be an option listed as default for centre point, switch it into model ref by picking any edges or something like that. It becomes the ref point for that view, so that even if u resume comps it will accomodate with ref to that point.
 
sharewithmani said:
MartinBooker said:
Me too !


Have you guys found the views get thrown around when this happens also ?


If anybody has a solution to this very irritating problem then I would be a happy man.
Click to expand...


Hi,


I accept with Ur Point but U can control Views from getting thrown.


The problem may occur when U resume UR suppressed features/parts, because Proe will place the views in drawing based on its centrepoint. When U resume the components/features it may grow more from the actual size of the model.


Solution:


When u place a view in DRW just go for prop & there will be an option listed as default for centre point, switch it into model ref by picking any edges or something like that. It becomes the ref point for that view, so that even if u resume comps it will accomodate with ref to that point.
Click to expand...


Top Tip. Thankyou for that sharewithmani.


Sometimes after placing a whole bunch of dimensions through the "show/erase" dialog I'll go back to this dialog to place the next lot and when it opens up, all the options are greyed out. As soon as I close this dialog, thats when the dimensions and sometimes views get scattered.
 
Lately in Wildfire 2.0 we've been having problems with the arrows calling out section views scattering. No dimensions or views move, just the section arrows. Hurray for 2.0!!
smiley32.gif
 
Have you tried "update current sheet" when your dims scatter? I've created a mapkey for this function because it happens so often... in 2.0
 
randypotts said:
Have you tried "update current sheet" when your dims scatter? I've created a mapkey for this function because it happens so often... in 2.0
Click to expand...


I get this with xsec arrows too but "Regenerate Draft" sorts that one out.


Doesn't sort out the scattered dimensions though
 
Has anybody ran into the problem of a associative note to a dimension blowing up really big? Well the dimension does not but the Tolerance does. the only way to bring it back to normal is to save the drawing and then update sheet.
 
I have also had the problem of everything in the show/erase dialog being grayed out, then having dimensions disappear after closing it. I fixed it by rebooting and starting up proe again. Not an elegant solution.


KWS
 
I have had the problem with dimensions scattering at least since 2001. I have complained up & down to PTC tech support with always the same answer: you need to have PTC recommended system, platfrom & graphics requirements. Well, this summer I finally did it and upgraded to all PTC certified workstations, graphics cards and whatever else I could find, and guess what, the problem still remained. Finally, this month they acknowledged the problem and filed an SPR (SPR1154988).


Following is more info from them (although the part about M140 not having any problems is not true - the issue is still there & I complained about it just today):


would like to mention couple of important information with respect to this issue.
<DIV></DIV>
<DIV>1. The issue is reproduced with drawings created in Pro/ENGINEER Wildfire1.0 drawings only. Once you save these drawings in Pro/ENGINEER Wildfire2.0, the issue can not be reproduced again on the same drawings..</DIV>
<DIV></DIV>
<DIV>2. The issue will occur while switching between different Pro/ENGINEER windows, ( that is from a model window to the drawing), by using the Windows Task bar. If the drawing is activated from the pull down menu # Windows within Pro/ENGINEER, the dimensions will not relocate.</DIV>
<DIV></DIV>
<DIV>As far as Wildifre2.0 is concerned, the issue is resolved in date code M140.</DIV>
<DIV></DIV>
<DIV>This is issue was already reported in SPR1154988.</DIV>
<DIV></DIV>
<DIV>However the issue is reproducible in pre-production release of Wildfire3.0. </DIV>
<DIV></DIV>
<DIV>I will check with the development whether this issue can be addressed in the pre-production release or we have to wait till the production release of Wildfire3.0 comes.</DIV>
<DIV></DIV>
<DIV>Please update to the latest date code of Pro/ENGINEER Wildfire2.0 ( M140 or later)in which the issue is resolved.</DIV>
<DIV></DIV>
<DIV>I will update you on the status related to Wildfire3.0 preproduction release</DIV>
 
One more thing, at first I thought this was a random occurance but I've found that it happens with parts with family tables. Modifiying a dimension directly in a family table and then immediately opening the drawing by clicking on the window makes the dimensions explode. If you have this problem, you should definitlely complain to PTC tech support. In my case, I complained for 2 years and they denied the problem existed until just recently.
 
We have had the same thing happen here also. I haven't experienced it, but my neighbor has several times. At our last corporate User's Group meeting I asked how many were experiencing this issue and about half of them raised their hands. So if anybody finds a solution, please, post it.


Thanks,


Mike Heath
 
You must log in or register to reply here.

Sponsor

Articles From 3DCAD World

Back
Top