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Helical cut problems!

sdoig

New member
heyho folks,


Trying to make a helical cut for the threat of a screw but continually getting the error message "unable to intersect part with feature". I'm following what my collegues do in the office and their cut works without any problems. Any suggestions what could be worng/being done wrong?


Ta all


Stuart
 

MOTO

New member
Try and changing the width at theroot or crestof the threadby .001 or so. Also try changing the depth or length some small distance as well.


Moto
 

snu661e

New member
whenever I have this problem, its just as burnsp said. Basically the cut is intersecting itself as it sweeps forward. Make sure your cut profile is per a standrad spec (ISO, BPT, whatever), and that your pitch matches that profile.
 

TrailBarge

New member
I got a new job and I've been in AutoCAD hell for awhile, but I seem to remember something like this happening to me as well. I'm going on rusty memory, so don't flame me too bad if I'm wrong.


First, you sketch your profile outside the part and cut in, right? This gives threads all the way in instead of a blunt thread at the beginning. Make sure that you are no more than one pitch (revolution) outside the part. We had a chamfer that made it so our profile did not start cutting for 1.125 revolutions and it gave us all sorts of headaches.


Second, some profiles (it was a buttress thread for us, oh my aching head) do not do well as a open profile. Try closing the two ends of the profile with a box in space... making sure that the box does not exceed one pitch, of course.


Third, in extreme situations, we would model the cylinder to minor diameter and use a helically swwept PROTRUSION to make the thread. Not elegant, but the kernel seems to handle these better.


I hope this helps.


P.S. Have you heard about the trick of taking the sweep profile and curving or angling it out at the head end of the thread? You can define the length of this sweep to be 2 1/2 pitches, which will give you the standard incomplete threads without a blunt end to the thread. Older kernels of Pro/E sometimes had a problem with helical cuts ending "hard" inside material.


Let me know if any of this works. I can only use solids vicariously while I fight viciously to get PTC in-house.
 

burnsp

New member
A couple of thoughts...


IfI'm modeling threads on a screw, I usuallystart thetrajectorya few threads below the screw tip and then sketch it up along the major diameter and curve it away as the thread nears the screw head. This simulates the action of pulling the tool away from the screw head so as not to cut it if you don't want a thread relief under the head. You can shape this curve anyway you want depending on the shape of your screw head.


For a double lead thread, I use only one thread profile but set my pitch to twice the normal value. I then copy and rotate the feature 180
 

burnsp

New member
An now for something completely different...why do all my posts (including this one probably) start one line down?


I see some post that seem to start at the top andothers that are one line down like mine. This thread has examples of both. Is it browser or OS related?


BTW, this postshows up at the top in the preview.
 

davidbullen

New member
Increasing the accuracy of the part in "setup" "accuracy" often works when this and other features fail for no apparent reason.
 

Zaki

Member
Hi stuart


can u put the part here in forum so I can check and repair the feature and put it back so u wil check what u missed.


Zaki
 

brchapman

New member
Looks like your not short of suggestions, but I thought I would give you something else to check. I believe you said you are sweeping the thread as a cut (this is good). I assume this is a standard 60 deg. thread. (doesn't really matter one way or the other). Are you aligning the top of your sketch with the edge of the part? I have found that if you make sure your section breaks outside of the part, you are clearly defining where you want the material to be removed. So, when you sketch your thread, cap off the top with a box or extend your thread section above the surface of the part. It does not need to be much. usually a few thousands works fine. Pro/E isn't always happy when you align edges during sweeps. The other suggestion has already been made, and that is to ensure your section is not intersecting itself. (Check the pitch and the section size.)
Edited by: brchapman
 

dcp2387

New member
I know this is an old post but I've had this problem in the past. I found another problem causer: whenyou're defining the section references, make sure to use the central axis and not the central plane. Sometimes when you reference diameters off the central plane, ProE tries to keep that dimension from that plane, which causes all sorts of problems.
 

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