[Jmooresshop]

Okuma Cadet with OSP5020L control,
I use the canned cycles through IGF. I don't know how to G Code anymore.
I'm trying to thread a 5/8-18 thread on CRS by 12 inches length of thread.
I have a partial profile insert by Mitsubishi. I am not having any luck. Inserts don't hold up.
I don't know how to make sure the insert is cutting on both sides either. Something to do with a 0, 30, or 60 degree approach.
Anyone got anything for me?

[deadlykitten]

far as i see, this is a 60 degrees thread ...

if you can convert that to mm, i can help you

is this correct ?
... diameter 5/16 = 0.3125 > 7.9375mm
... tpi 18 > pitch = 1.4111mm
... angle : 60 degress
... length : 304.8mm
... i guess it is an external thread ...

I have a partial profile insert by Mitsubishi.> why partial and not full ? what is the diameter before threading ? what is the diameter after threading ?

I don't know how to make sure the insert is cutting on both sides either.> do you wish for both sides to engage ? equaly ? 75 - 25 ? do you know what targets when sides are not equal engaged ? do you really wish for both sides to cut ? or just wanna get that thread done ?

Something to do with a 0, 30, or 60 degree approach. > yup, you can go 0 , 30 , 60 ... or even 2.123 degress

if i done the math correct, your thread is too long : 300mm for a 8diameter .. you need tailstock and steady rest ... how do you clamp and suport the part ? kindly !

at such length, machining on lathe is not effectvie; roller forming or buy 1 meter of such a thread bar and cut it to your need

if i was in the situation to do such a long thread, i would use attached tool, or a following steady rest

[Jmooresshop]

According to the Mits rep, if I approach at 30 or 60 I will be cutting on both sides of the insert. He seems to think this is what I need to do. It is a 5/8 diameter rod. I am using a live center.

[OkumaWiz]

Way to many unknown variables here... where are you at now for your cutting conditions? Are you experiencing chatter? Do you have good coolant flow and aim? What is your current tool life in # of pieces?

I would suggest around 450 SFM, (G97 of course) DOC of around .01, B59, and M73 M33 in the G33 cycle. This will give a zig-zag infeed and a reducing DOC as you near the bottom of the thread.

The threading defaults can be defined in your IGF parameters.

You may also want to check centerline of the tool or tool height. It is far too common to have the wrong shim under the insert and cut either above or below center.

[deadlykitten]

i was wrong ... i don't know why .. is not 5/16, but 5/8, so there is 15mm x 300

just tailstock won't deliver productivity ...

you must control and inspect each pass ... i would eliminate coolant and M0 after each cut and compare start-end position with middle ... in the middle will be bending problems

to reduce those, you must reduce cut depth ... with this, the tool will vibrate .. must find the propper balance

tool alignment comes into play at last passes ... if until there you have a nice surface, than so far so good

consider tool from post 2 ... will eliminate a lot of things ... if you wish, i can show you how to clamp that on a cnc lathe ...

[Jmooresshop]

Way to many unknown variables here... where are you at now for your cutting conditions? Are you experiencing chatter? Do you have good coolant flow and aim? What is your current tool life in # of pieces?

I would suggest around 450 SFM, (G97 of course) DOC of around .01, B59, and M73 M33 in the G33 cycle. This will give a zig-zag infeed and a reducing DOC as you near the bottom of the thread.

The threading defaults can be defined in your IGF parameters.

You may also want to check centerline of the tool or tool height. It is far too common to have the wrong shim under the insert and cut either above or below center.

I get about 3-4 parts before the insert breaks. Affirmative on the chatter. Good coolant flow. I will check the tool to see if it is on center.

[deadlykitten]

[ this post is just a comment ]

I get about 3-4 parts before the insert breaks. Affirmative on the chatter. Good coolant flow. I will check the tool to see if it is on center.

hello you mean 3-4 parts / edge or 3-4 parts / insert ? even so, you are lucky ...

Affirmative on the chatter.

where does this occur ( near tailstock, at middle, neat chuck ) ?
on which pass does this occur ?
how does your part looks between passes ?
can you inspect your part between passes ?

Good coolant flow + According to the Mits rep, if I approach at 30 or 60 I will be cutting on both sides of the insert.

your issues is not here, but because of L/D
so, if you try to change any of this, i guess you will still have chatter :
.... disable / enable coolant
.... change aproach angle to whatever value, and try ...

I don't know how to make sure the insert is cutting on both sides either.

that's simple ... use a marker and color your part between passes
generally, inserts cut on bought sides
when you start changing angles, it just cuts more on one side or another
to achieve cutting only on one side is tricky; even if you put a code for just that, than you hit into syncro precision

Something to do with a 0, 30, or 60 degree approach.

if you wish for a certain angle, for certain cut depth, i can help, but i need your thread drawging in milimiters, not inches

[deadlykitten]

[ this post is about my perspective on your part ]

your issues is stability, vibrations

[ insert ]

you said is partial, not full ... partial covers [ pitch_minimum ... pitch_maximum ]

inside this domain, where is your thread ? this idea is about insert nose radius, and so, if you are near " pitch_maximum ", than insert radius is too small, so you need to go with your insert deeper than a full profile also, if radius is lower than what you need, this makes the insert to behave more agresively comparing to a full profile ... thus, it will break faster; what radius is that insert and what radius do you need ?

another issues with partial insert, considering you have no more chatter, is that it cuts and also inputs plastic deformation near maximum diameter ... so you can't use them on soft material

however, insert on it's own is not a major player on your part

[ stability ]

thread is between za, and zb ... let's say za<zb, so tailstock comes at zb zm is at middle

[za] what is the distance between za and chuck front ? what shape is in between ?

[zb] is it pressure to low / to high ? put a dial gauge at zm and check play ... because part is long, you will have issues with this setup, because more force will increase stability near zb and decrease stability near zm, because material gets bended ...

however, tailstock on it's own is not a major player on your part

let's discuss this a bit :
...a) if length is short enough, you don't need a tailstock
...b) if it increases, than you need it
...c) if it increases a lot, than ... your case ....

it is possible to increase lenght from case b), but how :
... a normal tailstock just pushes
... try not to push your material, but clamp it instead, so :
....... clamp and push ( is like a tailstock with better grip )
....... just clamp ( just grip, with no internal tension among material axis )
....... clamp and drag ( grip with reversed internal tension ) > this allows better stability for thin materials ...

all above require some add-ons; i used the 2nd for a o20 x 400 ( 1inch x 15.7inches ), but for milling, not turning

this add-on can be converted for turning, but i don't think it will work for you ...

[ solutions ]

1) you need a following steady rest, or how is this it called ... to follow your tool and minimize material bending

2) cut only 0.2 .. 0.5, and after use the toll from my 1st post ... don't worry if you will have chatter, because you only need to guide that " tool " ... also, it may be enough to go with this low depth not on full thread length, but only near the tailstock

when thread teeth height is low, you must pay attention to how much you cut before the " tool "; for example, if you create a thead with an insert, and after that you want to use the " tool " over it, that tool might not work, because of " tool crafting issues " ... so instead of rotating free, there may be an elastic deformation, so that tool won;t rotate free, and also it wont cut ... you must create the proper cutting depth for it

3) do you have somehow a lathe with 2 turrets ? you can program the lower turret so to obtain solution1

[ alternatives ]

- send it to a colaborator
- if possible, send it to a classical machine
- leave the part / reject it
- put another operator on that part ... just kidding ...kindly !

[kevin0296]

At almost 20 times the diameter you would be lucky to even be able to take a light cut with a turning tool without chatter. I would imagine that in the middle of the stud the deflection alone would exceed the tolerance of the thread. You would need some type of a follower rest to have the best chance of making a good part by single pointing it. If the part is just the thread i would look into just buying some allthread.

[deadlykitten]

At almost 20 times the diameter you would be lucky to even be able to take a light cut with a turning tool without chatter ... into just buying some allthread.

yup, i also told him the same ... if you ask me, at 20times the diameter, he was lucky to post this thread

[OkumaWiz]

[ this post is just a comment ]


to achieve cutting only on one side is tricky; even if you put a code for just that, than you hit into syncro precision

Syncro precision is automatic - this is a thread and synchro is required. Your sync will be within tenths (or microns). Using the M33 zig zag will allow you to alternate between the left and the right side of the cutting tool. This reduces cutting forces significantly by reducing tool engagement. I suggested 59 degrees because this will further reduce tool engagement since the infeed angle will not match the tool angle so the edge of the tool will not be rubbing down the full edge. Your L/D is not really 12:1 since you are supporting it on both ends, so it is more like 6:1. This is still long and something like thread rolling would make this a breeze, but they are expensive so you would need to have high volume to pay for it.

The machine has this M33 capability for a reason...use it. 6:1 may be possible given the right conditions. The more your tool is engaged, the more cutting forces you have, much like using a wider groove tool. The wider it is the more prone it is to chatter.

You may want to post some code for us to evaluate.

Best regards,

[broby]

You only have to convert diameters to Metric in order to cut Imperial threads.
The G71 screw cutting cycle can handle Threads Per Inch very easily using the F & J commands.
You do not, and are better off NOT converting the TPI pitch into MM.
J is the number of Threads per distance F.
so for a 18TPI thread you would program F25.4 J18
the only proviso is that J values can only be a whole number.
So if you want cut 11.5TPI threads you need to do this: F50.8 J23
As for cutting on both sides of the insert, the best way of doing that is to use the Zig-Zag infeed pattern code of M33.
If you also specify the thread included angle of B60 this will allow the tool to cut inwards on a Zig Zag pattern while keeping the tool within the 60° angle.
See attached G71 instructions for more information on the various infeed patterns that the G71 cycle can use.

As for cutting a 5/8" 18TPI thread over 12" would be a challenge without some form of steady to prevent flexing and chatter.

Good luck.

[Jmooresshop]

Way to many unknown variables here... where are you at now for your cutting conditions? Are you experiencing chatter? Do you have good coolant flow and aim? What is your current tool life in # of pieces?

I would suggest around 450 SFM, (G97 of course) DOC of around .01, B59, and M73 M33 in the G33 cycle. This will give a zig-zag infeed and a reducing DOC as you near the bottom of the thread.

The threading defaults can be defined in your IGF parameters.

You may also want to check centerline of the tool or tool height. It is far too common to have the wrong shim under the insert and cut either above or below center.

Which page in parameters to change to zig zag?

[OkumaWiz]

I don't have a book for IGF here, but it would be the thread infeed parameters In IGF Parameters. I believe that M74 and M32 are default. i usually change to M73 and M33.

Best regards,

[deadlykitten]

if first pass is without chatter, than you may have a chance with different toolpaths ... otherwise, no way ...

does someone has a cnc lathe with following steady rest ? or is it "following rest" ?

[deadlykitten]

Which page in parameters to change to zig zag?

that pdf from broby should give you a hint :
... @ page 2 : G71 syntax
... @ page 5 : cutting modes ( zig-zag included ) + infeed paterns

also, consider attached examples ...

one more thing : G71 is a built in procedure that acts on its own ... not always delivers, but is a good start

material and fixture ask for specific regim; thus, G71 may need some trials to run

i suggest to try it on a shorter thread length, with good clamp, not with the tailstock ... once it works, change and go to your part ... like this, you are sure that you start with a G71 that delivers ,,, otherwise, you may run an improper G71 on a bending material

i don't use it because i can not control how it behaves ... kindly !

PS : i really wish you to solve your setup with G71 ... if so, please share your experience there is always plan B

[Jmooresshop]

Syncro precision is automatic - this is a thread and synchro is required. Your sync will be within tenths (or microns). Using the M33 zig zag will allow you to alternate between the left and the right side of the cutting tool. This reduces cutting forces significantly by reducing tool engagement. I suggested 59 degrees because this will further reduce tool engagement since the infeed angle will not match the tool angle so the edge of the tool will not be rubbing down the full edge. Your L/D is not really 12:1 since you are supporting it on both ends, so it is more like 6:1. This is still long and something like thread rolling would make this a breeze, but they are expensive so you would need to have high volume to pay for it.

The machine has this M33 capability for a reason...use it. 6:1 may be possible given the right conditions. The more your tool is engaged, the more cutting forces you have, much like using a wider groove tool. The wider it is the more prone it is to chatter.

You may want to post some code for us to evaluate.

Best regards,

I think this will help a lot. I just don't know how to go into the parameters and change it.

[Jmooresshop]

FOUND IT!!!

[deadlykitten]

to achieve cutting only on one side is tricky; even if you put a code for just that, than you hit into syncro precision

by that, i mean that you can not deliver nice flanc surface ( thread face ); syncro will generate sawteeth, with their height relative to syncro precision; small scale, of course :)

if someone really wanna go like that, than he/she :) may go as :
... in image 1 ; like this, sawteeth among orange line will be wiped out, and, except last pass, insert will cut amost on one side
... in image 2 ; this case does not change cutting direction, and insert will cut amost on one side, but a bit less than as in image 1 :)

well, feel free to experiment :)

Using the M33 zig zag will allow you to alternate between the left and the right side of the cutting tool. This reduces cutting forces significantly by reducing tool engagement. I suggested 59 degrees because this will further reduce tool engagement since the infeed angle will not match the tool angle so the edge of the tool will not be rubbing down the full edge.

hello mr Wizard >:D< ... and this is in image 3 :)

... to make it work, i guess you must declare B59 in G71 :) or not ?
... this " infeed angle < tool angle" technique, even if it " reduces cutting forces significantly ", will leave a very thin zone ( yellow - as shown in image 4 ) for the next pass, so the tool will cut only on one side, while the other side will mess with something <0.01 ( this is friction, not cutting, and will wear the tool ); to eliminate/reduce this fenomen, than 59 must be decreased, so to create enough cutting depth for the 2nd side, but this leads to increased cutting force ... this technique has a balance between [ reduced cutting force ] and [ friction ];

going as in image 2 comes with the same thing, only that this " friction " fenomen does not move from one side to another ... SECO recomends it as the "best method for cnc threading" ... possible, what can i say ?

I'm trying to thread a 5/8-18 thread on CRS by 12 inches length of thread.

what means CRS ?

Your L/D is not really 12:1 since you are supporting it on both ends, so it is more like 6:1 ... 6:1 may be possible given the right conditions.

in image 5, from left to right :
... 1) is a 5/8 10D clamped
... 2) is a 5/8 20D clamped + tailstock @ 0.5kn = i draw it vertically, and represent the equivalent force, as a bar o160mm*320mm; this leads to buckling even on lower tailstock thrust

... 3 and 4 are solutions to reduce this buckling, or if you wish " right conditions "
... 3) is the 2nd chuck ... i don't have a 2nd chuck machine, but i believe that you can push the 2nd chuck, so to act like a tailstock
... 4) is a puller, and so, it reverses tension direction, so will eliminate buckling

You only have ... Good luck.

hy broby, maybe i am wrong, but don't you wish for electronical manuals ? i think you scan&post too much :)

[broby]

hy broby, maybe i am wrong, but don't you wish for electronic manuals ? i think you scan&post too much

just goes to show how little you know at times...
Controllers of the OSP5000 series did not come with electronic manuals.
Whilst they might be now available (usually for a steep price as well) I do not have them for that controller.
Also, it should be noted that the basic programming methods for current controllers are very little changed from the 5000 series, so I suppose I could have extracted the relevant sheets that way.
Besides, I had this file on hand and did not need to go and scan it again.
If an answer can be give by scanning in and posting then why not? Better than not being helpful.