[daz59]

Hi,

I have a part that has an internal thread at one and and an external thread at the other, these parts screw into each other and have a hole on one side. currently when the parts are all screwd into each other the holes all line up down one side. without changing the tool offset or trimming the part a little to allow it to screw on another half rotation, how can I have one of the threads start 180degress from where it currently does.

Done on a cnc lathe, holes on side are drilled in a manual mill

My threading command for the internal thread is

G92 x28 z-9 I24 J3 K1
x28.2
x28.4 and so on

Thanks
Darren

[dcoupar]

You don't say what control yo have, but on some Fanuc's, you can specify Q180000 to shift the start 180°.

[daz59]

You don't say what control yo have, but on some Fanuc's, you can specify Q180000 to shift the start 180°.

Hi its a GSK controller.
I can use Q180000 with G32 but not G92.

G32 seems rather long to program, there must be a simple way of doing it?

Thanks
Darren

[txcncman]

Assuming the threads are the same lead, move the Z start point on one thread 1/2 the thread pitch.

[daz59]

Assuming the threads are the same lead, move the Z start point on one thread 1/2 the thread pitch.

Hi, thanks. yes I did that but in G92 it still followed the same thread.... I dont understand why it did.

So its 24tpi, thats just over 1mm per thread, I changed the start point of Z by 0.5mm, with the existing cut thread still in the lathe I recut the thread and it followed the old thread.

Thanks

[fordav11]

moving the start point should work. so if your G00 before the G92 is X50.0 Z10.0 the new start position should be X50.0 Z10.5

I assume you are putting a locking pin or something similar through the parts. the position of the holes needs to be calculated exactly on the circumference of the parts individually (using the C axis) in relation to the thread start point where it first cuts or you will get a rotational mismatch because your 2 parts are a different diameter. this would be very difficult to work out manually but if you use CAD software to work it out it should be relatively easy. Even with a perfect calculation this is still not a good idea because any minor variation on the machine with C axis backlash, X/Z backlash etc etc (i.e. mechanical variations) will result in a mismatch and the pin won't fit.

A better idea is to assemble the 2 parts and drill the hole through both parts when they are locked together.

[txcncman]

Hi, thanks. yes I did that but in G92 it still followed the same thread.... I dont understand why it did.

So its 24tpi, thats just over 1mm per thread, I changed the start point of Z by 0.5mm, with the existing cut thread still in the lathe I recut the thread and it followed the old thread.

Thanks

Should have been changed 0.02083", not 0.5 mm (0.01969"). Are you sure you changed the start point and not the end point? Post the before and after G-code.

[daz59]

moving the start point should work. so if your G00 before the G92 is X50.0 Z10.0 the new start position should be X50.0 Z10.5

I assume you are putting a locking pin or something similar through the parts. the position of the holes needs to be calculated exactly on the circumference of the parts individually (using the C axis) in relation to the thread start point where it first cuts or you will get a rotational mismatch because your 2 parts are a different diameter. this would be very difficult to work out manually but if you use CAD software to work it out it should be relatively easy. IMO this is not a good idea because any minor variation will result in a mismatch and the pin won't fit.

A better idea is to assemble the 2 parts and drill the hole through both parts when they are locked together.

Yes My code was
G0 Z20
G92 x28 z-9 I24 J3 K1

Changed to
G0 Z19.50
G92 x28 z-9 I24 J3 K1

The parts are baffles for rifles suppressors, off to one side of the main bullet hole there is a worm hole. each baffles needs that worm hole 180 degrees from the one under it. If a customer wants to buy extra baffles they need to follow that same alignemnt when they screw them onto their existing baffles.

Thanks

So the holes need to be machined on the same fixture.

[daz59]

Should have been changed 0.02083", not 0.5 mm (0.01969"). Are you sure you changed the start point and not the end point? Post the before and after G-code.

Hi, yes you are right but 0.5mm was close enough for a test.
Yes Chaned the start point, see my last pot for the code.

Thanks

[fordav11]

something does not make sense. the "I" indicates a tapered thread for a G76. G92 does not use I or J or K.
what control are you using?

if it is tapered you must be crazy if you think you can make two parts with tapered threads match the alignment of a drilled hole that is not done on the same machine at the same time using C axis. a taper with 10:1 ratio means a 0.1mm variation in X moves the Z (i.e. the mating part when screwed on) plus or minus by 1mm. so the rotation of the hole moves and the pin will never line up.
like I said, drill the hole after the two parts are locked together.

[txcncman]

Some thing wonky going on. Have you tried G76 multi-pass threading cycles on this?

[daz59]

something does not make sense. the "I" indicates a tapered thread for a G76. G92 does not use I or J or K.
what control are you using?

if it is tapered you must be crazy if you think you can make two parts with tapered threads match the alignment of a drilled hole that is not done on the same machine at the same time using C axis. a taper with 10:1 ratio means a 0.1mm variation in X moves the Z (i.e. the mating part when screwed on) plus or minus by 1mm. so the rotation of the hole moves and the pin will never line up.
like I said, drill the hole after the two parts are locked together.

No its a straight thread, I is the TPI, F for metric thread, J is Movement in the short axis in thread runout, and K is movemnt in long axis in thread runout.
I just setup the J and K as showen in an example in my manual, controler is a GSK 980TDb.

Drilling the holes after two parts are locket together doesnt suit my aplication. As I said in my other post, if a customer wants a baffle to add to his current suppressor I need to be able to supply him one that has that hole 180degrees from the existing baffle he has in his current suppressor (thinking into the future)

A simple fix for this problem would be to trim the part by 0.5mm so its screws on another 1/2 rotation, or change the offset of the threading tool.

The holes dont have to be exactly 180degrees apart, +/- 5 degrees is fine.

Thanks

[daz59]

Some thing wonky going on. Have you tried G76 multi-pass threading cycles on this?

Hi, No, how deos it differ from G92?

[fordav11]

G76 is essentially the same thing but only one line. you just specify the end diameter, end length and depth of cut (etc) and the machine works out the cuts automatically.
your control is non-fanuc so you would have to look up the exact format of G76 in your manual.

[daz59]

Hi,

Ok I got it to work with G92 by changing the start point.
Im not sure why that didnt work last time. I restarted the controller and it worked.

Thanks for the help

[txcncman]

Hi,

Ok I got it to work with G92 by changing the start point.
Im not sure why that didnt work last time. I restarted the controller and it worked.

Thanks for the help

Amazing.

[fordav11]

don't be too harsh on him. he's from New Zealand. they have more sheep over there than people