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Regeneration of Cross hatching

mvitez

New member
Does anyone know how to regenerate cross hatching on drawing? If I already have an X-section view and I change something on my assembly, the hatching is not good anymore. Then I change hatching in assembly mode and after regeneration of the drawing the hatching stay the some. If I then create that view again the hatching is o.k. If there is a lot of dimension, it is a problem to place them again.
 

gurveen

New member
Logically when you regenerate a drawing, hatching should regenerate but sometime in assembly drawings it won
 

mvitez

New member
I followed your instructions but I didn't get any message. I must say that I don't have Pro/Assembly license, only the Foundation. Could that be the reason?
 

mvitez

New member
I need to say that I have tried at least a hundred times to regenerate my assembly and drawing on every possible way and nothing happen. I always need to change the hatching manually on drawing (if there are not a lot of changes) or to place the view again after I change hatching in assembly mode. It is a problem when I have around 300 parts in assembly.
 

dflockton

New member
This may be a really stupid thing to say, and forgive me if you've already tried it, but try going to View\Regenerate View\All Sheets.
 

donha

New member
If a component changes size in an assembly, you must choose Regenerate/Model/Automatic or choose the component by name. The safest bet is to use Automatic. Next, you must regenerate the view or all views. Even after this is done, you sometimes have to choose Regenerate/Draft. You should never have to redimension and as a rule of thumb, dimensions on a drawing should be driving (driven by geometry) rather than created dimensions, another subject for another thread :)
 

mvitez

New member
Thank you all for your time but I tried all of that and nothing helps. I think that I need to accept that there is no solution for my problem.
 

mvitez

New member
I tried but it doesn't help. Regeneration just doesn't work...grrr.. When I create another view like the one that I can't regenerate the hatching is o.k. I have this problem since I'm working with ProE (2 years) and you are not the first that I asked about it but it looks like nobody can solve my problem :-(

Thank you anyway.
 

donha

New member
There is a bug in Pro/E if the section cuts through a part that creates a small segment, the crosshatching will not show. This normally occurs when you have a cross section going through complex geometry. You will need to do one of two things: 1: Change accuracy so the cross section does not have a segment smaller than your accuracy or 2: move the cross section by .0001, if you have the luxury to do so. I have been on Pro/E since 1991 and the above is the only crosshatching problem I have seen. When this happens, the crosshatch will not show at all.
 

mvitez

New member
I think that you don't understand my problem. I have hatching on my X-section but I'm not satisfied with the angle (e.g. it must be 45 deg to the edge) or spacing. It means, I already made my X-section view, then I change angle and spacing of X-section (but in assembly or part mode, not on drawing) and after that I can't regenerate my hatching on my X-section view (on drawing). If I then place another (the same) X-section view the hatching is ok.
 

donha

New member
What you do in the part/assembly does not change the drawing if the drawing view is already created. I beleive the option of changing the hatching in the part/assembly is there for viewing purposes in the part/assy. If you have your view created on the drawing, highlight the hatching, right click and choose properties. I just verified that indeed after the view is created, the hatching spacing does not get changed if you change the hatching in the part.
 

ProFishent

New member
donha is correct. It's just like saved orientations and explode states, they do not update either once you have placed a veiw. Pro/E does this so that you can make changes that will apply only to new veiws, and not mess up your existing drawings.
 

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