What's new
What's new

Help chatter while machining a shaft (CNC lathe).

I'll attempt to clamp even tighter down tomorrow when I setup for the other side. I'll also reduce the tailstock stickout as little as possible as the turret has this huge table that kind of forces me to have the tailstock shaft stick out almost completely. the setup is pretty similar to this for the EN24T (pictured is EN19T) had a lot of issues getting this to also gie me good cuts without chatter.
View attachment 434338


Now that I seen your pic above, the first thing that I thought of then was quill stick-out.
That needs to be as low as possible!
Also, are you able to clamp it down tight (cinch) once engaged?

Is your finished part one diameter all the way?
If it was a different size on the tailstock end, I would want to use a second tool for that end, and it would need to be mounted towards the back end of the turret top plate.
This would allow you to choke your tailstock up another 4-5", and would likely make a whale of a difference for you!
If it's gotta be all one turn, then that makes that rough.

BUT - if it is all one turn, why not just rough it in and toss it on a centerless grinder?


---------------------------

I am Ox and I approve this here post!
 
Now that I seen your pic above, the first thing that I thought of then was quill stick-out.
That needs to be as low as possible!
Also, are you able to clamp it down tight (cinch) once engaged?

Is your finished part one diameter all the way?
If it was a different size on the tailstock end, I would want to use a second tool for that end, and it would need to be mounted towards the back end of the turret top plate.
This would allow you to choke your tailstock up another 4-5", and would likely make a whale of a difference for you!
If it's gotta be all one turn, then that makes that rough.

BUT - if it is all one turn, why not just rough it in and toss it on a centerless grinder?


---------------------------

I am Ox and I approve this here post!

I'm going to try and reduce the quill stick out as much as I can tomorrow and see if that helps. as for the tailstock it has 2 levers ( 1 to lock the quill and prevent it from moving - I turn it has hard as I possibly can once the rotating center is pushed in - this is the last step),a turning wheel (to turn the quill in and out - I turn this as much as possible until it doesn't allow me too - 3rd step), the 2nd lever is basically like a 2nd clamp to secure the tailstock to the bed (2nd step) and lastly there's a nut and bolt that I tighten as much as I can to secure the tailstock to the bed. Also no most of the long shafts I machine are gear shafts and similar so they have variable sizes some with undercuts etc if all of them were one size through I would've attempted to put on the running steady but it's such a tedious task when I have all the various sizes the EN24T has 3 different sizes back end is 100mm dia (0.00/-0.03mm) 74mm long, 2nd size is 70mm dia (0.00/-0.03) with total length being 580mm if I recall correctly, and the las size is 60mm dia (0.00/-0.03) 80mm if not mistaken (this has been the simplest shaft I've had to machine in terms of varying sizes) I hope this image I made quickly shows the shape as I don't have the drawings with me atm.

1711569403174.png
 
With that holder you have a negative back rake angle. It’s for roughing. To finish to a clean surface change that to zero or even positive. The side edge angle should be bigger. Speed: the material can be turned at up to 90 m/min. or 300 sfm, so at 100 mm diameter 286 rpm max. Depth of cut not over half a millimeter or 0.02". Feed: defined by corner radius, diameter of work, and surface quality. Overlapping after a revolution gives smoother surface. There are wiper inserts that have a straight length behind the cutting corner leaving almost a mirror finish. Coolant very important.

If machine too weak for the part, better grind/have ground between centers.
 
Use a positive rake insert- - back in the old days, a common shaft turning insert was a KNUX, lots of side rake to curl a chip, but great for reducing chatter. The ones we used were Sandvik. Looks like they are still available.

 
With that holder you have a negative back rake angle. It’s for roughing. To finish to a clean surface change that to zero or even positive. The side edge angle should be bigger. Speed: the material can be turned at up to 90 m/min. or 300 sfm, so at 100 mm diameter 286 rpm max. Depth of cut not over half a millimeter or 0.02". Feed: defined by corner radius, diameter of work, and surface quality. Overlapping after a revolution gives smoother surface. There are wiper inserts that have a straight length behind the cutting corner leaving almost a mirror finish. Coolant very important.

If machine too weak for the part, better grind/have ground between centers.
Hi now that I'm reading this I've come back with some updates:

1. I reduced my quill stick-out by a further 10mm (anymore will cause the turret to run into the tailstock). I attempted to take a further cut with the DDJNR2525M-1504 still had chatter issues.

2. decided to change tool a kyocera DTGNR2525M-16 with a TNMG160402GP with a doc of 0.5mm (1mm overall) with no chatter at recommended values for the insert (Vc = 220, Ap = 0.5, f = 0.11) this gave an RPM of 700, feedrate of 77mm/min, chips are forming almost "c" like patterns and best of all no chatter and super smooth finish (max recommended Ap is 1.00mm so I will attempt my next cut at that and if no chatter at present I'll be satisfied just sucks that each cut would take roughly 7min to complete.

1711611721340.png


3. Had the TNMG insert not worked I would've attempted to use a WNMX060408 MM TT8125B insert from Taegutec with the TWNLR holder (only ever used it once)

1711611834075.png

I appreciate your input and will check if I have any tools and inserts that have either a positive or zero rake angle (never really paid attention to it) I'll definitely also look into some wiper inserts for finish passes.
 
Use a positive rake insert- - back in the old days, a common shaft turning insert was a KNUX, lots of side rake to curl a chip, but great for reducing chatter. The ones we used were Sandvik. Looks like they are still available.

Funny that you talk about KNUX inserts there's a old poster here in the office that have them on along with other inserts called GTN, TPMR etc and I'm talking this poster has turned yellowish old doubt the company still exists that supplied them over here. I'll check to see where the closest Sandvik supplier is here as we do have some old toolholders from them for the manual lathes but I don't think they have been used for a long long time
 
My two cents — if you will be raising the feed, adjust by ±20 mm/min until chatter is minimized
Hi this is something I attempted to do the funny thing is it would cut smooth for like 3-4mm and then back into chatter city I attempted to also adjust feedrates and would temporarily remedy the solution
 
I'm going to try and reduce the quill stick out as much as I can tomorrow and see if that helps. as for the tailstock it has 2 levers ( 1 to lock the quill and prevent it from moving - I turn it has hard as I possibly can once the rotating center is pushed in - this is the last step),a turning wheel (to turn the quill in and out - I turn this as much as possible until it doesn't allow me too - 3rd step), the 2nd lever is basically like a 2nd clamp to secure the tailstock to the bed (2nd step) and lastly there's a nut and bolt that I tighten as much as I can to secure the tailstock to the bed. Also no most of the long shafts I machine are gear shafts and similar so they have variable sizes some with undercuts etc if all of them were one size through I would've attempted to put on the running steady but it's such a tedious task when I have all the various sizes the EN24T has 3 different sizes back end is 100mm dia (0.00/-0.03mm) 74mm long, 2nd size is 70mm dia (0.00/-0.03) with total length being 580mm if I recall correctly, and the las size is 60mm dia (0.00/-0.03) 80mm if not mistaken (this has been the simplest shaft I've had to machine in terms of varying sizes) I hope this image I made quickly shows the shape as I don't have the drawings with me atm.

View attachment 434359


OK then, so - with this design, you CAN rig up a tool on the other side of your turret top plate, and likely reduce quill stick-out to zero, or at least 4" less, and that will make a huge difference!

With that tool - then you can run that small diameter, and then change over to your other tool(s) to run the rest of the part.


----------------------

I am Ox and I approve this here post!
 
With that holder you have a negative back rake angle. It’s for roughing. To finish to a clean surface change that to zero or even positive. The side edge angle should be bigger. Speed: the material can be turned at up to 90 m/min. or 300 sfm, so at 100 mm diameter 286 rpm max. Depth of cut not over half a millimeter or 0.02". Feed: defined by corner radius, diameter of work, and surface quality. Overlapping after a revolution gives smoother surface. There are wiper inserts that have a straight length behind the cutting corner leaving almost a mirror finish. Coolant very important.

If machine too weak for the part, better grind/have ground between centers.
He's already having issues with chatter, no need to introduce more tool pressure into the equation.
 
no need to introduce more tool pressure into the equation
The more positive the rake angle the less pressure between tool and work. Under negative angles the tool scrapes, at positive angles it cuts. Material removal happens more easily but the tool becomes weaker because narrower between chipping surface and back relief. At a certain point you want to change from hard but brittle carbides to tough steels.
 
OK then, so - with this design, you CAN rig up a tool on the other side of your turret top plate, and likely reduce quill stick-out to zero, or at least 4" less, and that will make a huge difference!

With that tool - then you can run that small diameter, and then change over to your other tool(s) to run the rest of the part.


----------------------

I am Ox and I approve this here post!

I wish I knew what you meant by hooking it up to the other side of the top plate, only way I can think you mean is that I hook it up on the side of the turret instead of on the inside slots (as if I would be hooking up a left hand tool on the turret or as I would put on a boring bar? -) If that is the case I'd like to definitely give this a try when I get something similar to do.
 
w
He's already having issues with chatter, no need to introduce more tool pressure into the equation.
Would this still be a factor even if its a finishing pass? (I'd assume one would leave no more than 0.5 to 0.3mm before the final cut for wiper inserts?)
 
I usually say sharpness of the edge, positive rake for steel that wiill file, and the toolbit/insret angled/set so cutting forces will swing the bit/insert away, not deeper into the part.
I understood the first but up until the file part but the rest I'll have to do more reading on to understand better
 
I don't know what it takes to doo this on your machine, but on my Hardinge / sub-spindle machine, I have pockets for tools in the back side of my top plate. See where my #3 is?

DSCN3551.JPG

I had some shafts to run last year that took every ounce of daylight that my machine had available, but I didn't have enough Z to run like you are trying to. So I put a tool in one of these rear pockets, and I worked the first step of the part with that tool, and then switched to the regular tool pockets to run the rest of the part.

I didn't see any pockets like this in your turret, but you can likely get some bolt-on holder that would allow you to put a tool back there. Or - worst case scenario, you take a few hours and make one yourself.

But the value of this is that you wouldn't need to run your turret as far back, and thus - you can scootch yuhr tailstock right on up tight, and not have to deal with the limitations of that quill.


------------------

I am Ox and I approve this here post!
 
UPDATE:

Firstly I'd like to thank everyone that gave some form of input and tips to this thread all of it is much appreciated as it helped me get this part done and I think it would be a disservice not to give a run down on how I came to eventually finish the part.

In future I will look for a toolholder/ inserts with positive rakes as mentioned here unfortunately I am not too well versed with machining yet to grasp all the differences inserts make for machining certain materials.

1. Used initially a 0.4 DNMG to machine the first side of the part down to 99.98mm with the use of the steady as I didn't have much meat to play around with to get the sweet spot - too much chatter when using this tool for this respective job - RPM was @ 500 and Feed @ 100mm/min, with the use of the fixed steady it worked perfectly but initially would prefer doing without the steady.

2. I switched from using a 0.4mm radius DNMG insert with the respective tool mentioned earlier in the thread to a NMG160402GP with its respective tool named earlier in the thread with a DOC of 0.5mm - I will attempt to use this tool and insert next time also when I am machining down to 100mm (0.00/-0.03mm) with the initial 2mm to be roughed out by the DNMG to get rid of the outer shell hardness.

3. Speed and feed used to avoid chatter initially was done using the recommended values as the insert suggested this gave me SFM @ 200 , AP = 0.5, f = 0.11 (calculated and got 700 RPM @ a feed of 77mm/min) I tried pushing the limits by using a DOC of 1mm and instantly encountered chatter so I reverted back to 0.5mm DOCs this was good for about the first 108-90 mm diameters then chatter started to become present now I don't know if this is shown in some book or if I just overcomplicated it but this helped me understand whatever since I was getting the cut and finish I was looking for and had a sweet spot for RPM and feed I did not want to tos around figuring it all out again so I worked on a ratio which was 9.09 rev/mm = (700 r/min)/(77 mm/min) I used this as my arguement for every 10mm e.g 9.09 = (600/x), x = 72 mm/min and this worked up until I got to 68mm diameter where I had to change the speed to 400 RPM and 174mm/min finish was rough and not satisfactory but to speed up time I let it run until 61mm I had to once again reintroduce the fixed steady to do the finish cut of 59.98 mm.

4. Tallying up all the time I spent machining this part (program writing, testing, setup and diagnosing problems, measuring etc.) I came to just shy of 23 hrs which I think is a bit too long for my liking for such a shaft I'd like to see if I can't better this time by minimizing the setup times by if needs be only using the steady once at 61mm, use a different tool which will allow me a more stable cut at a deeper DOC for roughing (e.g using the knux inserts reducing stailstock). If I can get it to machine the part finish at just sub 8 hrs I'll be ecstatic.


SIDE NOTE: I will say though I am having minor issue where over 500mm distance I have a particularly weird thing that happens on the part the first 150mm (closer to the tailstock) when taking a reading at e.g 20mm and at 140mm with the micrometer I get exact readings (maybe about 0.002 to 0.005 mm difference) but then readings at eg 160mm and 560mm I have difference of 0.02mm (cutting exactly the size I want at 160mm and at the back closer to the chuck I sit with a -0.02mm difference) which luckily still falls into the required tolerance of 0/-0.03. anyone experience this before?

Once again thank you all for providing possible solutions to this problem I look forward to attempting some of them when such as job lands on my table again.
 
I don't know what it takes to doo this on your machine, but on my Hardinge / sub-spindle machine, I have pockets for tools in the back side of my top plate. See where my #3 is?

View attachment 434955

I had some shafts to run last year that took every ounce of daylight that my machine had available, but I didn't have enough Z to run like you are trying to. So I put a tool in one of these rear pockets, and I worked the first step of the part with that tool, and then switched to the regular tool pockets to run the rest of the part.

I didn't see any pockets like this in your turret, but you can likely get some bolt-on holder that would allow you to put a tool back there. Or - worst case scenario, you take a few hours and make one yourself.

But the value of this is that you wouldn't need to run your turret as far back, and thus - you can scootch yuhr tailstock right on up tight, and not have to deal with the limitations of that quill.


------------------

I am Ox and I approve this here post!
Now that I see what you meant the turret I have unfortunetly does not have such slots but a few handy tool holders were provided with it so I more than likely will be able to do something like this just need to figure out how to as you said worst case scenario would be me making one which I would have no problem doing. Thanks man very nifty trick might just do this for the E19T shaft I have next on my table (luckily just once size right through)
 
SIDE NOTE: I will say though I am having minor issue where over 500mm distance I have a particularly weird thing that happens on the part the first 150mm (closer to the tailstock) when taking a reading at e.g 20mm and at 140mm with the micrometer I get exact readings (maybe about 0.002 to 0.005 mm difference) but then readings at eg 160mm and 560mm I have difference of 0.02mm (cutting exactly the size I want at 160mm and at the back closer to the chuck I sit with a -0.02mm difference) which luckily still falls into the required tolerance of 0/-0.03. anyone experience this before?


Sometimes when you are chasing tight tols on long parts, you need to "map" it out.

"U" is your friend.

G1 Z-4.5
U-.002 Z-9.
U.002 Z-13.
Z-16.

I don't know your control, but I suspect that it has U?
Of not - you can obviously X it, but U is nicer for tapers...


---------------

Yuh gotta doo what'chew gotta doo, if you wunna be who you wunna be!
Ox
 
Sometimes when you are chasing tight tols on long parts, you need to "map" it out.

"U" is your friend.

G1 Z-4.5
U-.002 Z-9.
U.002 Z-13.
Z-16.

I don't know your control, but I suspect that it has U?
Of not - you can obviously X it, but U is nicer for tapers...


---------------

Yuh gotta doo what'chew gotta doo, if you wunna be who you wunna be!
Ox
To add to what Ox said that is completely true by the way. Also look at TS pressure. Sometimes at the beginning of a cut it is fine, but if you take a fair amount of material off it will bow some.
 








 
Back
Top