http://www.mcadcentral.com/creo-drawing/16411-hlr-quilts-secti-n-view.html
"You need to cut the cross-section through "Model & Quilts". You will have to re-create your cross-section to select this option. And make sure you have "Remove quilts in total x-sec" set to yes in your DTL file. Then you should be able to seld "HLR for quilts".
Hope this helps."
http://www.eng-tips.com/viewthread.cfm?qid=289407
"Try implementing the config.pro option
HLR_FOR_QUILTS YES from Tools
- Options
Check the following posted by user alibahadir at
Here is the solution for that offered by Ptc
Hidden line removal is known as not working in X-section views containing quilts which usually come with vendor parts.
In order to enable the HLR settings for X-section views (by the view settings or by the default settings with config.pro option 'hlr_for_quilts' set to YES), there are two requirements:
1. the dtl (drawing config.pro) setup option 'show_quilts_in_total_xsecs' MUST be set to 'yes' (the default is 'no')
2. the cross section MUST be created using the option 'Model & Qlts' for the cross section definition
Michael"
This is in third angle projection; the welds ringed in red should be hidden, however I want to keep the welds which SHOULD be visible, rather than hiding them all.
In the end, prior to pdf-ing it, I hid the welds in the model and manually drew in the weld fillet in the right hand view where they should be visible. A bit of a dirty work around, and not something I should have to do!
Okay, this is still annoying but might work for you.
Nothing changes the line style view specific for a fillet weld that I tested. You only want it to show up that way in specific views, so changing the model's weld line style isn't a solution.
I went into the sketch mode in the drawing, toggled the parametric sketch option on and projected the weld edges I needed as hidden and once created (while still highlighted) I changed them to the Hidden line style. I then went through the drawing layer per view routine to hide the weld in that view.
When I changed the weld parameter, the drawing edges updated but when I added an additional segment, of course, I had to create the new edges again by projecting them. Using intent edges may solve this but in general, you get the idea.
Not being able to change the line style of the weld edges is somthing that appears to be a major oversight on PTC's part. Simon, have you considered asking tech support how PTC expects such a feature to be managed in drawings by opening a support case? If you have maintenance, you have every reason to get their input.
This is what I came up with... also notice the light weight line in the left side view for the weld... I suspect it should be the same line weight as solid edges.
I'll be darned! Yes, this also hides the quilts in front of the cross section view if they are hidden.
Unfortunately, it also erases the ones that should be visible.
I cannot weigh in on the welds when it comes to standards. I just make sure it is clear on drawings. Ground seam welds are always a challenge when it comes to the fab drawing and subsequent assemblies. Since this is only a rare requirement, I model the weld as a separate feature in an assembly.
