Results 1 to 20 of 20
01-11-2006, 02:59 AM #1
Another project I am working on are some tensile specimens for my department here at school. I need to make about 250 of them. I know how to set up and run the machine (Gildemiester CTX 410 with less than 20 hours on it) However, I don't know much about turning steel. Basically I am just looking for some speeds and feeds.
The parts are 7" long, 3/4" diameter and is a dogbone with the center being 2" wide at 1/2" diameter with .375" radii bringing it back out to the stock dimension. I am running a 50 someodd degree neutral tool for roughing and a 35 degree for finishing. Though have toyed with the idea of just running the 50 degree one and saving the tool change even though the machine changed tools in the blink of an eye. I find my finises to be better with the separate finishing tool.
I am getting stringy curly chips. Should I push it harder. Or just take it easy.
DOC and Feeds and Spindle speeds would be greatly appreciated to see if I am in the right ball park.
01-11-2006, 03:22 AM #2
I'd leave the DOC where it is, but increase the speed to around 800sfm and the feed to .012 ipr for starters. You have to push 1018 pretty hard to get the chips to break. A .010 feed will usually break them when turning with a O or 5* lead angle tool, but if your diamond is in the neutral position then its 27.5* lead angle will be thinning the chip, hence the need for a heavier feed.
01-11-2006, 03:32 AM #3
800sfm would be running about how many rpm on the .5" diameter?
01-11-2006, 05:48 AM #4
800 SFM on .5 dia. = 6111 RPM. Yes 1018 will be stringy. A lot depends on the specific toolong you have available. Negative rake tooling will help, as will the style of chipbreaker. As suggested more feed on the rough turning tool, up to .015 depending on your tooling. At 6000 rpm the tool is gonna FLY across that part I haven't made any tensile test specimens since tech school. We had to polish the .500 diameter and the radii at the ends...supposed to stop the specimen from breaking at a tool mark in the finish. But that was on flat belt SBL's. Your machine should be capable of a good enough finish "as turned". Stay with the separate finish tool to hold the size and finish. Using a .03 nose radius tool and .01 feed should yield a 125 finish. You probably want better than a 125 so .005 to .007 range ... even less if you are using a .015 nose radius.
01-11-2006, 10:04 AM #5
How do you figure the tool life will be at that speed?. I can only run up to 5000 rpm though. I'll play with it. But thanks for the advice.
01-11-2006, 03:22 PM #6
Was never involved in any sort of "production" runs, but I'm guessing a couple inserts will do your whole batch.
01-11-2006, 03:24 PM #7
I finish 1018 around 1000 sfm. Since you are limited to 5000 rpm I'd run at a constant rpm of around 4500 for the whole part (for finishing). You'll likely see surface finish better at the larger diameters than at the smaller diameter. I use a steel grade insert...Sandvik VNMG 331 PF 4015 with good tool life.
Rough at about 600 sfm with the feed rate suggested (.015).
01-11-2006, 07:56 PM #8
Was going to start cutting them today but am having problems getting the tail stock to engage. I am all programed and ready to go. Other than the fact that the tail stock will not register as engaged agianst the part. When the tailstock is in this state it locks most functions of the machine out. Basically the only M code that will activate is M54 which retracts the tailstock. So after a few hours on the horn with a DMG applications engineer (whom I met when he set up the machine) I have made some headway with the tailstock. I can at least get it to come out of alarm and sometimes reference into home position. But as far as getting a program to run with it engaged I have not had any luck yet. Hopefully service will be coming to visit soon. It's too bad really becuase a service guy was just here this morning (before I had the issue with the tail stock) working on a sprint 20 that we have on show for applictions testing.
12-14-2016, 11:38 PM #9
I know this is an old one, but it's all I'm finding on turning 1018.
Machine: Haas SL30
Material: 2" 1018 Solid Round
Insert: Iscar CNMG 432-GN IC8025
Feed: Tried 0.008 to 0.02
RPM: Tried from 800-3400, also tried CSS
DoC: Tried 0.075, 0.100 & 0.125
Roughing angle: 0
I'm having a tough time getting chips to break and it just wads up into a stringy mess and does bad things. They'd chip fine if it were just a couple straight cuts to the OD, but it tapers to a 60deg point like so > and it starts wadding up after the first couple passes. It does seem like more rpm is the way to go, but I've had a couple big chips in the insert at higher rpm and I'm hesitant to get aggressive with it again.
Not seeing how to upload files, but the 'back to square one' code is below. Any advice would be much appreciated.
(PROGRAM NAME - Expendable Tip P2)
(TOOL - 4 - 80 DEG. INSERT CNMG-432)
G97 S800 M03
G0 G54 X1.8424 Z.086 M08
G99 G1 Z.056 F.01 M31
G0 Z.0404 F.01
X2.0641 Z-1.7524 M09
G0 X10.0 Z5.0 M05
12-15-2016, 05:36 AM #10
Make sure you use an insert with the proper chip breaker for the feed range and depth of cut you intend to use. Just slapping any old insert on is not good enough.
12-15-2016, 07:01 AM #11
Philabuster liked this post
12-15-2016, 08:06 AM #12
Lose the G97 and go with G96 constant-surface speed. I may be wrong, but I think the GN chipbreaker on that insert is kind of heavy. Try moving to a lighter chip-breaker if you can.
12-15-2016, 08:15 AM #13
for stringy material like 1026 tube, DOM and 1018 I run Walter CNMG431 in WPP10S grade with an MP3 chip breaker
1018 around 1000sfm .012 feed .06 depth of cut (Haas ST-10)
These inserts break chips in DOM like a dream as well I run a bunch of parts in 2.5"x .375 wall DOM with the WNMG431 version on a 1" bar breaks chips like a dream and leaves an awesome finish.
corndog liked this post
12-15-2016, 08:41 AM #14
Anyone notice a 10 year old thread got bumped?
alliancefab liked this post
12-15-2016, 08:59 AM #15
12-15-2016, 09:20 AM #16
12-15-2016, 11:14 AM #17
7" long and 3/4 to 1/2" dia
feeds and speeds assume rigid parts, since that is a long length to dia ratio you will get chatter if you push to limits.
long stringy chips some material make long chips easy. often material is selected that makes nicer chips. real bad material often chip breakers and different feeds and speeds do little to stop long stringy chips. programming feed changes of
often the feed change rate will break chip. or a flat out pause delay of a second periodically often works too. some cnc have a chip breaking cycle
12-15-2016, 11:25 AM #18
Apologies if posting in this one is against the rules/etiquette. Definitely not selling anything!
ISCAR Cutting Tools - Metal Working Tools - CNMG-GN : 5593939 - CNMG 432-GN
I'm not seeing the IC8025 grade. If the grades are numerically close in type, this would be the closest: ISCAR Cutting Tools - Metal Working Tools - Grade : IC815
It's a 30hp machine. I can get chips to break on the very OD with DoC from 0.050 to 0.100, but it seemed worse going beyond that. I agree it cuts like butter....just a giant string of butter that likes to wad up and ruin parts/inserts. I could probably run all day if I added a couple/few interrupts to manually remove wads, which I may have to do in order to run today and tomorrow.
CNMG432 MP3 WPP1S Grade Carbide Turning 476111 - MSC As overpriced as MSC is, they have a warehouse nearby and parts get here quick. I'll give these a shot.
Can someone explain how changing the roughing angle may help, as well as what a safe angle is to use that doesn't cause the backside of the tool to interfere with the material?
Again, apologies for posting in an old thread and thanks very much for the replies.
12-15-2016, 12:32 PM #19
12-16-2016, 06:45 PM #20