[CJdave]

Trying to put a 1"-8 thread on a 1" 1018 cold rolled bar. I am using a Iscar single point partial profile uncoated threading insert. I am having a terrible time with galling and can't get a clean thread. Looking for some suggestions as to what I am doing wrong! running at about 400rpm, but I tried 300, 500, 600, and still the same. HELP!
Thanks
Dave

[djr76]

Can you change your lead (in-feed) angle? Thats a coarse thread also, so slow rpm, light depth of cut and some heavy duty oil might help.

[HuFlungDung]

Do you have to use C1018? It takes a lot of speed to make that come out shiny. Dark sulfer bearing cutting oil will also assist in smoothness of the thread, it still may not come out bright and shiny.

The partial profile insert may also be pointier than ideal, forcing you to cut deeper than necessary, and the sharp tip is easily damaged, leading to surface galling. You could perhaps hone or grind a bit of a flat on the insert. A coated insert may resist chip built up edge too, but you really need more rpms to take advantage of that. If you cannot get above 350 to 400 SFM, then you won't get a bright surface.

[Konrad]

1018 is sh..ty stuff for threading,....but it should work, using HSS tooling with a little more rake works better,
Sometimes I even use it on the sh..ty 316 SS.
I find carbide don't give you enough rake for material to flow out properly.
And yes, a small radius on the tip helps, necessary on coarse thread.

Konrad

[juergenwt]

How many parts? What machine? How long are the parts and how long is the thread?

[CJdave]

I think I have the wrong anvil under the insert. i am going to try and get a 2.5 degree instead of the 1.5 that is in there now.
Machine is a millport 1740 with a centroid control. I can run faster and harder but it didn't seem to get better with speed. I am running flood coolant (valcool VP tech). Thread is 1.75" long and parts are chucked up as close to the chuck as I can get. I have 50 pcs to run, and this job will repeat in the future, so finding a good solution for fast and repeatable results is worth the time and money spent.
thanks for your suggestions.
Dave

[Gearsau]

Dave
How many passes are you taking ?

Is your machine CNC ?

You are running at 400 RPM, so, that equals 33 m / minute ( 108 SFM)
That speed is too slow for carbide , even if it is uncoated, and if your machine is CNC, I would suggest that you try to run at least 1,000 RPM.

Program your first pass to be approx. 0.012" ~ 0.105" deep ( these imperial numbers get confusing)

Alternately, if you cannot run any faster, I would suggest HSS.

Carbide needs the speed to operate correctly.

I must look at the chart regarding the shim seats as well.

Hope this helps.

Regards from Australia ...............Peter G.

[CJdave]

OK,
Thanks for the replies! I ground a small radius on the insert tip, and pushed my surface feet up to around 250 (950 rpm) and Wow! nice clean threads no galling, first pass is at .017 last pass is at .002.
Thanks for the help guys!

[pdoherty]

Ain't it nice when the solution gets the job done faster?

We just finished up a job threading a couple hundred bolts with an M48 x 4 in 4140 QT, 24" away from the chuck.

We had a huge center hole (used a 1" dia. center drill) for the tailstock, but were getting chatter as we got about 5" away from the end (the thread length was about 6").

We were screwing around in the 100 to 500 rpm range, trying all sorts of things and finally got frustrated and ran one at 900 rpm. Problem solved, loser job now a winner.

[g-codeguy]

We were screwing around in the 100 to 500 rpm range, trying all sorts of things and finally got frustrated and ran one at 900 rpm. Problem solved, loser job now a winner.

One thing I discovered a long time ago was if chatter doesn't go away at slow rpms go faster. Even if the chatter still doesn't go completely away at the higher rpm, the threads will look much better. The distance between the chatter marks becomes finer as you increase the rpm. You may need a loop to see the chatter. Also try not to make any spring passes. Often makes chatter worse. Keeping a load on the tool can help.

[Brandhoff1234]

I neglected to mention that i'm working for a small job shop. I kinda gotta make things work. I agree it's not the right thing to do but I have limited resources. But you are right...I haven't done alot of threading. It's prob been at least two years since I've chased a thread. I've mostly done alot of profile work. Some threads but nothing tight. This is my first " J" thread ever and the first time I used a Johnson Gage.

I really appreciate all the information and the help.