pipe tap

[beamer]

Does anyone know how to put in a pipe tap? I am using wildfire2 and I thought it would have been part of the hole comand. Does it have to be sketched in.


Is this another Pro/E short fall?

 

[dr_gallup]

No tapered threads in WF2. I have attached an NPT.hol file you can use but it will show as a straight thread.
2006-03-01_172707_npt.zip

 

[beamer]

Thanks!


Do you know if WF3 is going to address this or will it be PTC as usual

 

[Dell_Boy]

I am a little surprised you are using the hole function to put in a
pipe thread. I think that every time I have wanted a female pipe thread
it has been on the inside surface of an already existing revolved cut or protrusion
because the solid body is virtually never a block type solid. If I was
going into a valve body I would probably use a UN-O thread so there was
no chance of distorting the body due to over-tightening.



As for not having exact taper threads; who cares. The machinist will
read either BSPP or BSPT in the annotation and make the necessary
changes.





DB



P.S. it could be worse. In Solid Edge, if you want to put any female
imperial thread into a metric part, you have to have the minor diameter
accurate to about 5 decimal places or the thread won't build



Edited by: Dell_Boy

 

[dr_gallup]

I agree the taperer or straight is just a visual thing but it bothers me that something so simple can not be shown properly. The purpose of a drawing is to convey information and if the thread callout is tapered but it is shown straight that causes confusion.

I generally add a spot face to a curved surface before applying a hole feature. Pro/E can not handle screw theads in standard hole features on curved surface properly either, the intersection is wrong.

 

[beamer]

Thanks!


I have been using a revolve cut. The reason I am asking is because I also use Solidworks and you can insert a NOT threaded hole.

 

[brchapman]

I must agree with dr_gallup. It is very annoying to have a side view of an external pipe thread that shows a tapered OD but a straight thread. The machinists in my shop know what it is, and have no problems making the parts, but it still looks bad. As far as whether or not to use pipe threads, I would have to agree that o-ring boss seals (I assume that is what Dell_Boy means when he says un-o) are far superior to pipe threads. I have used them for years on hydraulic systems, gear boxes, clutch housing etc. Unfortunately though, There are still lots of applications that my products go into thatuse pipe threads. So until everyone converts, we will bestuck with having to use them.

 

[Dell_Boy]

a picture of a UN-O can be found at



http://www.bareco.com.au/files/hydraul2001/hy3.htm


I believe that all relevant thread parameters should be specified
in the annotation which can easily be shown in the plan view. I
generally don't specify minor diameter or drilling depth, thread class
etc as I have confidence in the machinist getting it right. How the
thread looks in a sectional view is a purely cosmetic thing and as long
as the hidden line removal works correctly, I'm happy.



If you are really that worried about looks you could put a patterned
tapered revolved cut in to form the thread (though I would not
recommend using a helical cut) and define a this as a UDF or use
feature/copy/different model to copy between parts rather than
re-create it each time.


You said it yourself; the machinists know what it is and the
fundamental point of a drawing is to convey the information to the
target audience. Mission accomplished.



The advent of CAD has enabled designers to include a level of detail
never considered in drawing board days. Sometimes that detail helps
avoid confusion which is great but putting in detail because is looks
nice is probably overstepping the mark.





DB







Edited by: Dell_Boy

 

[timjr]

2006-03-04_130549_npt_tap.gph.zip


I like to use this udf for creating NPT pipe threads. It doesn't actually show the threads, but it does have the taper.


Tim

 

[Israr]

Dell_Boy,


you are right but ptc should look toward improving it in the next releases.


Israr

 

[brchapman]

Dell_Boy


There are actuallyseveral types of ORB (O-ring boss seals). The most popular here in the states are straight thread o-ring boss seals as defined by SAE J514 and ORFS seals (O-ring Face Seals) defined by SAE J1453. Of course it seems like everyone has their own standard as can be seen by looking at some of the ISO and DIN ORB Specs.


I believe the fittings shown @ http://www.bareco.com.au/files/hydraul2001/hy3.htm
as UN -O-ring are actually Straight Thread O-Ring Boss fittings per SAE J514. I say this because the thread sizes next to the ORB plug shown match exactly to the J514 fittings:


1/2-20 UN = -4 (1/4" Tube); 9/16-18 UN= -6 (3/8" Tube) etc.


I hear exactly what you are saying about the pipe thread situation being only a cosmetic issue. Again, it does not worry me, it is merely an annoyance. With all of the power Pro/E has, I am just a little surprised they have not addressed this yet. While I have cut threads using a helical sweep when I felt the thread was a dominant feature on the part, it is obviously not an option for most threaded features (And I am, and always have been perfectly satisfied with the straight cosmetic threads).


I too, describe my threads with annotations of course. Ialways specify minor diameters and drill depths for internals, as well as major diameters for externals. I also always specify thelead in chamfer dimensions and under cuts (if required). Details are what separate great part fit and finish from merely good part fit and finish. When done correctly, the part cost will be also be less because no deburr will be required.


While I have some very good and experienced machinists working for me, I cannot be surethe one making my part on any particular daywill have the same understanding of thread geometry and fits that I do. Plus, this ensures the part is made exactly the way I want it, no surprises. Also, the way todays (greedy?) management is always looking to outsource our work, it is nice knowing all part geometry is explicitly defined.


You are correct about the level of detail and accuracy Pro/E provides. There is no better design tool out there.


BC

 

[dr_gallup]

How the
thread looks in a sectional view is a purely cosmetic thing and as long
as the hidden line removal works correctly, I'm happy.



The advent of CAD has enabled designers to include a level of detail
never considered in drawing board days. Sometimes that detail helps
avoid confusion which is great but putting in detail because is looks
nice is probably overstepping the mark.



DB

Correct representation of a tapered pipe thread was a piece of cake with a drafting board. Is it too much to ask for a "high end" CAD system to be able to do the same thing, quickly and easily without UDF's and workarounds?

Of course there are technically superior solutions to tapered pipe threads but if you want to draw one it should be easy and correct.

 

[Dell_Boy]

I wish you luck with your request for taper pipe threads however I
don't see it happening very soon as no doubt they will get lots of
complaints that hidden line removal in assembly sections aren't working
because of the difficulty in getting major and minor conical
"diameters" to be exactly coincidental which is a REQUIREMENT for
parallel threads.



Personally I would be much happier with hole functionality if I could
edit a thread (rather than having to use edit definition) to change the
principal (major/minor) diameters. That way the thread is modifiable
from anywhere including in a drawing.



While we are at it, I would also like to be able to put principal
diameters into a family table so the small version of the part can have
four M6 holes and the big version can have 6 M8 holes.



Also I would have an immediate use for being able to directly dimension
a hole orthogonally from a single axis which would be useful for
features like mounting 4 bolt flange bearing units or SAE pads and
front flange mounts on hydraulic and pneumatic cylinders.



To do these three things, I currently have to resort to using cut
features and a separate thread. It would be nicer to do it in one go.



I can see why you need to specify your holes more completely than I can
get away with. Because of the nature of my work, we often have to give
our machinists half-finished drawings because they need to start making
parts before we have finished designing them.





DB



Edited by: Dell_Boy