Help creating an SPL Thread in Pro-E WF3

[Tazlear]

Hey there,


I am trying to create a thread with the sketch pattern (or thread pattern) being best described as having two circles connected by tangent angled lines onboth sides.


View attachment 4643


I am new to Pro-E, but have created a few threads with no problems at all. This one however is truely ruining my opinion of Pro-E's flexibility with options. I have tried multiple helical thread cuts where I would separate the feature in two, I have tried Helical Sweep Protrusions, and neither worked. I started my 3D solid modeling work in SolidWorks, and know that the design above works there, as well as a few other options tocreate what I want. I am trying to work with my new employer and see if Pro-E is worth keepingas long as thesefeatures are possible to be created in short, quick steps. These featuresare primary in most of our products (not to these dimensions of course). How can I make this thread work???Sweepprofileline is located on the outer edge of the feature, diam. .53, extending .1 fromboth sides to create the thread fully through part. Pitch is .125.Don't bother with a full round radius feature, itonly crashes the system every single time. I am at a loss, anyone have a solution? (fewer steps, the better)


P.S. I am close to suggesting this site to create a location where sketches for working features (as well as incorrect details for feature designs) can be viewed, I learn best by example personally, and figure many others do too.
Edited by: Tazlear

 

[dr_gallup]

Your helical sweep is self intersecting as your profile length is equal to your pitch. You might want to create a spiral curve by equation and try sweeping along that. Not sure if it will work with self intersection, just know that's what we had to do before they made the helical sweep feature.

This site had an area for sharing files but the powers that be hid it. Actually the files are still there but you can only get to them with a clever google search, not by navigating the site itself.

 

[Tazlear]

Dr_Gallup,


I understand what you meanabout the flaws of self intersectinggeometry I have in my sketch, this profile was the last one I created after jumping back to see the different options I had to play within SolidWorks. I just kept the sketch to showon the forum so I couldgive visualization to my sketch explanation.I am going toattempt your suggestion today and give a reply on the outcome.


Anyone else with suggestions? I would greatly appreciate the help. Otherwise I hope improvements to my situation were made in WildFire 4 since my boss is either going to buy that, or switch over to SolidWorks! Let the race begin!

 

[Tazlear]

Ok, so I tried the helix formula with a sweep, but I must have done it wrongor it may just notwork.


I also looked into the option hammerpe suggested, but the thread has to meet the dimensionalmeasurementsI gave, and I noticed you changed the sketch profile to .001 shorter. I don't know if that was an accident, or if you made your pitch the same length, but I leave it any other way than I originally sketched it...


Then, I started playing with threading only half the part. Itried to mirror & rotatethe feature but found it was only possible to mirror the feature, not both, and didn't find an option to rotate it. I finally got it with doing the procedure twice, once each half. made the profile the same length as the pitch, and made the sketch profile go all the way across the part. The only problem I have now is that the regeneration takes a while and I need to impliment a design table to the finished part. May be on the verge of crashing. Wish me luck!


View attachment 4664

 

[dakeb1]

See the attached part: -


2010-09-24_042752_db-helical.prt.zip


A Helical Sweep Cut with a .125" pitch works fine for this profile in WF3, but you MUST draw the section ENTIRELYinside the solid material, not outside it, or you will get the error "could not intersect part with feature". You can cut the material away later so the thread goes right through. ProE will allow the other endto extendbeyond the material, so you only need to cut awaythe startend.


You don't need the .05" deep rectangle, just draw a line coincident with the profile of the material.


Alternatively (just out of interest) ...


A Variable Section Sweep (as a solid cut) will also work, along a curve with the cartesian expression (where r = radius of material and n = number of threads): -


x=r*cos(n*360*t)
y=r*sin(n*360*t)
z=n*t*.125



...but you have the same problem of having to create at least PART of the sketch inside the solid, and I think additionally for a VSS you will have to keep it partially inside the solid atthe far end too, meaning you will have to cut both ends afterwards for thread run-out.


You will have to set the Section Plane Control to "Normal to Projection" and select the section reference as theaxis of cylinder, or your section shape will gradually rotate normal to the curve.


Also, you will have to change your part accuracy from the default .0012 to .0006 to avoid self intersecting errors (edit/setup/accuracy).
Edited by: dakeb1

 

[Tazlear]

Hey dakeb1, I can't access the file becauseI am using WF3. I think your file is a different version. I have figured out what you meant, I appreciate the help.


So I had everything working fine with the double sided thread, until half way through my project, the thread on one of the sides decided to randomly switch directionand I went throughall knownmodifying options to try and correct it, but nodice. Back to square 1.


I tried the helical sweep withcutsketch inside of material and having to maintain that for both sides, so overall sketch detail isshortened and by twice thepitch so now I need to compensate by adding material for both sides. That does work, but like you said, I'm turning a one step process for other programs into a 2 or 3 step process.


1. Cut Thread Detail.


2. Revolve or Extrude Cut excess ends at pitch distance or whatever excess that exists on one side.


3. Or Revolve Cut excesson both sides if not constrained by other surfaces and distances.


This adds to my calculating time, adds tothe complexity of my design approach, adds to my design time, takes away from my efficiency. Is this really the most efficient and simple way to create this thread in Pro-E?

 

[dakeb1]

The model I provided was created in WF3.

I don't know why Proe will not allow this type of cut to transition
from space into solid, possibly due to the way the program handles
the graphics I guess.

It is a minor problem though, and not really an extra step as you
need to calculate the cut end length anyway. Just allow extra stock
length and develop the part in exactly the same order you would
machine it: e.g. cut stock, machine thread, face off.

This method will produce a robust model.

Cheers,

David