We're having issues with getting threads to display properly in specific cases. It occurs when we have an assembly of parts where the machining operations occur at the assembly level and threads are applied. In a drawing of that model, the threads do not display correctly in a section view. The available options (to stick with ansi) std_ansi and std_ansi_imp_assy and related drawing setting (hlr for threads etc)and config files don't allow us to get it right (at least none of the combinations we've tried, and I believe we've done them all). The ansi option shows a line through the view (across the part) representing where the thread starts and ends - not correct. With std_ansi_imp_assy, nothing shows at all. But here is the weird part: If I go into one of the part models that later get a thread applied at the assy level, and create a cosmetic thread....even if so small it is not easily visible....suddenly the threads applied at the assembly level show up correctly in the drawing. If anyone can explain this to me I'd appreciate it. We just want our cross section view of an assembly to show a hidden line representing the minor diameter of an OD thread and major diameter of an ID thread when the cosmetic thread is applied at the assy level.
To reproduce. Make two simple cylindrical parts. Assemble them together coaxial and mated at ends (imagine you're welding or brazing blanks together that then get machined). In the assy, create assy cuts that represent some turning operations that might be done. Make one or two that create the area where a thread will be applied. Apply the cosmetic thread. Now make a drawing of the assembly with a view looking at the profile (not end on where the cylinder would appear as a circle), make that view a full or partial section. With "std_ansi" set as the thread display standard in the dwg setup file, you get the lines going across the dia of the model - not good. With "std_ansi_imp_assy" you get nothing at all. Now go back in and create a cosmetic thread in one of the cylinder parts at the part level. Go back to the drawing and presto, all of the threads are displayed correctly.
I've tried this with Wildfire 4 M220 (what we're on) and Creo 2 M060 (what we're moving to soon). In fact, I don't recall it ever working correctly.
Thanks for any tips
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I opened a call with PTC tech support about this issue. The fix was to change the drawing setup file option "crossec_type" from "new_style" to "old_style". The tech comfirmed this is a known issue with an SPR filed against it to be fixed in a Mcode update of Wildfire 5 (Creo Elements Pro 5 I'm assuming).I'm assuming the fix will also be implemented in Creo 2. Theproblem is we had changed this option to "new_style" to address and issue with drawings of some complex assemblies totally failing to display a section...so fix one issue, recreateanother.