Segment dimensions and breaks

Does anyone know how i can shrink, break, reduce cable segments for a MFG MFG drawing while keeping the original dimension? When ever u use cable breaks the dimension on my drawing also reduces.





~Rob

Disclaimer: I've been using Pro/CABLING for about a month...


It was explained to me that the break is used to indicate where a wire/cable/bundle would get looped up to take up the specified amount of slack when manufacturing the harness. So, having the dimension you added change makes sense. Roughly, a break in manufacturing is for manufacturing and is not intended to be the same as a break in a drawing (perhaps they ought have called it coil instead of break).


So, what do you do? Well, if you show dimensions for the segment one of them will be the original overall length. Or, if you want to override the dimension value and set it as you please, you can replace @D in the dimension text with @O (letter not number) followed by whatever you want the dimension to say.


I did the latter (override), but really dislike the basic premise. Now I have some automatically updated dimensions and some not! *ick* Maybe on the next drawing I'll get a little better at this.


Cheers,


-kyle

Rob,
In the drawing pick the view you want to break. In properties use Visible Area/Broken View. This maintains the length.

jef

Hi rob,


i got your problem i need some more clarification so please send snap shot of your problem for better under stand after that i will give solution for these problem.

I cant take snapshots due to company and Gov rules. basicly, ProE wont allow the user to use the "Break Segment" tool without also making the true dimension shorter. On the other side of this, the ProE drawing package does not break segments of harnesses, only vertical or horizontal planes. This forces me to make vehicle size harnesses really small and blow up a ton of detail views rather than just shrinking the segments for drawing clarity.


The other option is to use the break tool and override the dimension however, this is not possible due to company rules.


Just looking for a solution to shrink harness segments for drawing clarity while keeping ture dimensions.

Not sure why I didn't think of this before. It is still a bit of a hack, but the dimensions are driven so perhaps it would still pass a check of your rules.


In my case I can't just show the dimension for the segment because I want it to be more than just that segment (includes a parent segment and connector). Anyways, the idea is to show the overall length dimension (it is a ref) for the segment that you want to break, then use relations to sum that dimension with whatever other dimensions you need (maybe TOTAL_DIM = a5:1 + a6:1). Of course, you can't directly put @O&TOTAL_DIM in the dimension you want but you can do @O with a space after it then do an offset note and put &TOTAL_DIM[.2] in the note ([.2] as an example for 2 decimal places).


Of course, this is still a hack (albeit driven by the original dimensions) and may not even be useful if you want the sum of non-shown dimensions, but hopefully it is useful somehow to someone.

Thanks for the info. This solution will be helpfull in harness that do not have connectors. such as solder cap wires to plug into and amp and other applications. As for the solution with connectors, i had submitted an enhancement request to PTC. Maybe one day they will create a cosmetic break tool.

One more thought to deal with connectors... a measure feature in the assembly! So, in theflat harness (I did it in the 3D, but either ought to work) measure the dimension from the connector face to the bundle (or wire ends or...) then set the measure to a feature and save it. In the drawing, set the appropriate model to be shown in the model tree (so you can see the saved measure). Now create the relation (as above) using:


INSERT->FROM LIST...->Look in FEATURE-> click on your analysis feature->click on button to insert into relation


Above copied from: [url]http://www.mcadcentral.com/proe/forum/forum_posts.asp?TID=36 519[/url]


It's round about, has to be maintained, etc... but it is driven from the model. Of course, follow the note and overridden dimension approach I described before.


One can only hope that PTC will answer your request so that we can achieve this without all the overhead.

I hadn't done much with relations in drawings before so I didn't realize that drawings don't have relations. This would explain why we can't reference the dimensions made in the drawing... Anyways, I put my measures and relations in the flat harness assembly (the assembly in the .mfg file). Also, it seemed that I had to click the execute/check relations button to force recalculation presumably since the drawing wouldn't trigger a regen of the flat assembly.