Results 1 to 8 of 8
01-11-2006, 01:59 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, 02:22 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, 02:32 AM #3
800sfm would be running about how many rpm on the .5" diameter?
01-11-2006, 04:48 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, 09:04 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, 02:22 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, 02:24 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, 06:56 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.