how to create NPT pipe threads?

I'm sure you've already tried the conventional things: for example, you tried 'Insert>Cosmetic>Sketch' and that doesn't help and you tried 'Insert>Cosmetic>Thread' and that's only for UNC/UNF/ISO threads, not pipe threads. So, there's no (I repeat, NO BUILTIN) way to produce pipe threads, cosmetic or otherwise. Or, maybe it's MEs who recognize bolt threads but not pipe!?! I haven't yet determined the source of the insanity (especially in a system that does routed systems, including piping {oh, that's the ticket, you're supposed to buy pro/piping to get pipe thread!! boy, am I brilliant}) but I'm bettting it's some footshooting theory about making money.

So, here's an alternative (in Pro/e parlance, a workaround): Copy your tapered surface and offset it inward the representative depth of the thread. As the cosmetic thread is actually a surface, this will look like one in the drawing.

This config.pro option will allow you to create tapered pipe threads in Pro|E:

ALLOW_UDF_STYLE_COSM_THREADS

I had to provide one of our mold designers with this info a few years back when he was wanting to create some User-Defined Features for waterline holes.

Ron M.

Sorry about not including the value for this particular config.pro option. Just set it to a value of 'yes'.

Ron M.

Well, Ron, be nice if this worked, but I'm not sure what it's supposed to do. If it's supposed to produce a a straight cosmetic on a tapered surface, it works fine. And then it lets you look up all those numbers about tapered pipe thread no one remembers like pitch, major/minor diameter, depth. (I'm sure, if you do this every day, you've got it down. And you need to cuz Pro/e's no help!) When this enables UDF style cosmetics, is there, perhaps, a little more to this, like possibly needing a library of UDFs for pipe threads and somehow integrate this into cosmetics, maybe even going so far as to have the UDF provide the parametric information for the thread note. Well, Ron, I'm not getting any of that just by setting ALLOW_UDF_STYLE_COSM_THREADS to Yes. In fact, I don't see any difference at all. BTW, if you want a gander at the old style interface based on the socalled Menu Manager and it's essential junkiness, just go to 'Tools>UDF Library'. These MM menus were present for all file functions: Dbms? List? Anyway, Ron, I think we're missing some key pieces of the puzzle here, not just the value of the option.

Thanks for the constructive feedback David. And I agree with you 100% about the old Menu Manager still being used for the UDF Library functionality.

Regarding the config.pro option that I posted not really bringing anything that advantageous to the table, that is also true. Good catch on this one, and I most certainly apologize to the group for not having reviewed some of my old documentation and e-mail trails before posting. I wanted to try and help the original poster out with his issue based upon some things that some mold designers and I had worked on together in the past. Until I reviewed some dated documentation today when I stopped by the office, I had forgotten that we actually ended up doing something a bit different as the ultimate solution for their taper threads issue. My mistake. Losing my memory! :-) But here was my intentions:

1) Create the Hole feature using the Sketched option and of course taper the sides. 2) After having set the config.pro option ALLOW_UDF_STYLE_COSM_THREADS to YES, add a Cosmetic>Thread feature by interactively entering the Thread Depth and Thread Diameter values and ignore the other UDF-related garb. 3) Then just edit the section sketch for the Revolve feature and use the Parallel constraint to snap the outside sketch entity to be parallel to the silhouette edge of the tapered hole.

While this does work, the same type of revolved surface feature can be created with the Revolve functionality(check the Surface icon on the Dashboard) and would serve the same purpose. Quilt Hidden Line Removal for drawing views would still work if applicable to the user/company's processes for drawing documention. Providing of course that they are still relying on

2-D drawings like a lot of us are. And a Cosmetic>Thread feature could still be redefined to have the side section sketch entity modified to be parallel to the sketched Hole feature's tapered, silhouette edge even without the config.pro option that I posted being set to YES. This is where I jumped the gun, and I most definitely want to apologize for spreading some bad, Pro/E-related information on this one. Just wanted to help and ending up causing confusion. Once again, I'm sorry for this as well as the brevity. I was posting from home and didn't have any of the documention from the past accessible to me.

By the way, the mold designers ultimately ended up making their own sketch Hole UDFs and they included Revolved Surface features to represent their threads cosmetically. They set these up so that they could show their dimensions from the UDF and the dimension's annotations were parametric and all. I did a search in PTC/USER Exploder for tapered pipe threads and found another thread where someone was suggesting that the config.pro option ALLOW_UDF_STYLE_COSM_THREADS be set to YES in order to do the modification of the Revolve feature's side sketch entity. At least that makes me feel

*somewhat* better about screwing up in public! :-)

Oh yeah, David, I'm glad to hear that someone else out there doesn't remember all of those thread pitch, major/minor diameters, etc. That too makes me feel a little better.

Thanks again for the catch on this one. I'll have to make sure that I do my background research more thoroughly before posting next time.

Have a great weekend everyone. What's left of it.

Ron M.

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Here's where I'm completely lost: I don't get any "UDF-related garbage", for some reason; even with the option set to yes, the interface stays the same old Menu Manager list ~ Thread Surface, Start Surface, Thread Depth, Major Diameter and Note Params. Should it be a different interface? look different? let you do something like model the thread surface or ask you for the name of a UDF to use and show you the UDFs in pro_group_dir. I don't think I'm seeing what you're seeing, Ron. And I'm wondering if there isn't some other option that needs to be set to make it work

Well, I guess you're getting to sketch the cosmetic profile. I'm going to have to try this on a different machine. At no time does it offer the option to sketch a profile. I'm also thinking that the advice I gave to begin with (doing an offset surface) sounds a lot easier than all this rigmarole. But, I'd at least like to see what I'm missing.

Hey, I'm not sure you did "screw up" except for making ANYTHING in Pro/e sound simple and easy, especially anything involving UDFs.

It's why we depend on the intelligence built into computer programs, where Pro/e in some respects shines and where in others it falls flat on its face, leaving the users to do the heavy lifting. For example, wouldn't it be great, when you wanted to do your waterlines in the mold package which you paid a pretty penny for, it interviewed you on the configuration, input and output sides, cooling rate needed, then let you preview some layouts. You hit the ok button and they're done, with pipe threads, (come on, really, you can't make water lines without pipe threads, who in their right mind would sell a specialized package to do molds which absolutely need water lines, give you water line functionality but not finish the job with pipe threads? makes no sense) with plugs, with nipples or quick disconnect couplers. Now, if PTC wants to brag about productivity features and program intelligence, the above, comprehensive approach would give them strong bragging rights. If you were sitting down right now to program an enhancement to the existing mold package, this is what you'd be aiming for. We're having this discussion only because that's missing.

Hi David, Hope everything is going well for you today. Mondays can be tough sometimes! At any rate, I made time to check into this issue some more this morning at the office, and below are my observations.

When the config.pro option we have been discussing was set to YES, and I chose Insert>Cosmetic>Thread, an Open dialog box appeared with two folders listed. One was named External and the other was named Internal. After double-clicking the Internal folder, two new folder names appeared. One was named Blind and the other was named Thru. When I double-clicked on the folder named Blind, Pro|ENGINEER issued the following message in a new dialog box:

'The UDF tolerance standard is missing. The UDF cannot be updated since the reference part is not available. Click OK to continue without tolerance standard compatibility, or click CANCEL to abort placement. '

So I clicked on OK and moved forward. Then Pro|E brought up the good ol' MM style UDF prompts for Same Dims, Scale, etc.--just like it does when placing any other UDF. And of course it issued a message about the UDF being in INCH units when these types of prompts appeared on the right-hand side of the screen. I just chose Same Dims and continued to answer the prompts for Thread Surface, Thread Depth and Thread Diameter. Pro|E just created a revolved surface with straight sides and did NOT give me the opportunity to sketch a tapered section. This was no different than the last time I tried it. But here's where it gets confusing, thanks to PTC. The software reports the feature type as being different in certain places. Here are four examples:

-Feature>Info shows the Cosmetic-Thread feature as being a Revolve

-Model Tree shows it as a Revolve

-Hovering cursor over it in the main graphics window brings up a pop-up feature description tag that says it is a Thread feature

-Doing a Layer Properties listing for the Surface layer lists it as being a Thread feature

So in two places Pro|E defines it as being a Thread feature and in two other places Pro|E lists it as being a Revolve feature. Huh???!!! Why is that??? Anyhow, again, all you end up with is a non-tapered, revolved surface feature that is represented in the Model Tree with the regular Revolve icon. When the config.pro option ALLOW_UDF_STYLE_COSM_THREADS is set to NO, the resulting Cosmetic-Thread feature is NOT a Revolve and is represented in the Model Tree as a true Cosmetic feature with no section sketch that can be edited to have tapered sides that are parallel to an existing sketched Hole feature's tapered, silhouette edges. This latter finding is actually contradictory to what I previously stated in an earlier post where I had read in a different config.pro file, which as it turns out, had the same values set as the previously used one.

With this said, David, I would prefer your originally suggested Offset Surface methodology. Even if the user ends up having to trim or extend their Offset Surface feature's end(s) to achieve their desired results, it's still probably the least hassle of all the different approaches. My number two choice would probably just be a revolved surface feature's creation. Either of these two methodologies seem to be acceptable. And of course there's always the option of creating a UDF of a sketched Hole feature with tapered sides, coupled with a revolved or offset surface feature. Dim.s could be set up for parametric annotations and shown in a 2-D drawing if required.

Like you said in your last post, we're having this conversation because of a lack of core functionality that should already be available for the big bucks that we pay PTC for such add-on modules as Pro|MOLDESIGN. Perhaps some of the newer mold extension products actually have tapered pipe threads features in them now and I'm just behind the times.

Thanks for your help and input with this issue!

Best regards,

Ron M.