Tapping

[Palafox]

I hope you can help me.

Im going to tap a stainless steel part in my CNC machine.

Can you point me to a table or chart that can show me which feedrate and rpm should I use?

Thank you very much. Best regards.

[ryanduc]

hi
what size the tap & how depth to go.thanks

[DAB_Design]

As a general rule at work, we always use the following to determine feed and speed for taps.... Feed always equals 9.9ipm and RPM is 10 times the pitch.

So for a 1/2-13 tap, we would use 9.9ipm and 130RPM. In some instances we will use a dividing/multiplying factor. Sometimes slower for hard metal and faster for soft metal. But make sure you multiply/divide both RPM and feed (for example - 19.8ipm and 260RPM for a 1/2-13 tap, or 4.95ipm and 65RPM for titanium). Dividing is only done when problems with breakage can't be remidied by other means.

Make sure to use tapping fluid. Coolant will somtimes work on aluminum, but any hard metal really should use a dedicated tapping fluid.

[Palafox]

Originally Posted by ryanduc what size the tap & how depth to go.thanks

I will be tapping nuts with a Ø1/4"-28 and a 5/32" depth. The thread will go from one side to the other.

[Palafox]

Originally Posted by DAB_Design As a general rule at work, we always use the following to determine feed and speed for taps.... Feed always equals 9.9ipm and RPM is 10 times the pitch.

So, in my tapping, I will be using 9.9ipm and 280RPMs, right?

Originally Posted by DAB_Design So for a 1/2-13 tap, we would use 9.9ipm and 130RPM. In some instances we will use a dividing/multiplying factor. Sometimes slower for hard metal and faster for soft metal. But make sure you multiply/divide both RPM and feed (for example - 19.8ipm and 260RPM for a 1/2-13 tap, or 4.95ipm and 65RPM for titanium). Dividing is only done when problems with breakage can't be remidied by other means.

In this case the material is stainless steel. It is not hard as titanium but the chips are very hard to break. What do you think if I use 4.95ipm and 65RPM?

Originally Posted by DAB_Design Make sure to use tapping fluid. Coolant will somtimes work on aluminum, but any hard metal really should use a dedicated tapping fluid.

I have always used coolant. Its hard for me to change the fluid because it is a big tank and different materials are machined in a same day. I use a sintetic MOBIL coolant. It will work?

Originally Posted by DAB_Design Feed always equals 9.9ipm

If Im correct ipm means "inch per minute", right?

[DAB_Design]

Yes, 9.9ipm (inches per minute) and 280RPM.

If you want to cut it in half, it would be 4.95ipm and 140RPM. But since you are only tapping 5/32 deep, I don't think it will really be necessary.

As far as tapping fluid, it is usually sold in small containers. You apply it directly to the tap or hole. Since you have a through hole, you would apply it to the tap. It's not something you would have to replace your coolant with. And it is easy to clean up, so contamination of your coolant would be minimal if at all.

Are you using a reversable tapping head, or does your spindle reverse?

[Palafox]

Originally Posted by DAB_Design Are you using a reversable tapping head, or does your spindle reverse?

Since this is my first tapping project, I dont know what do you mean by "tapping head". But it is not an excuse. Im going to study and search what that means.

Im going to use a SANDVIK COROMAT tapper in a MAS CNC. The MAS CNC is controlled by and 2100 Acramatic control.

The MAS CNC can spindle in clockwise and counterclockwise direction.

I believe that my tapper is a "floating tapper" because the end moves in and out. The rigid tapper is the one that doesnt move, right?

As you can see, Im a newbie.

[DAB_Design]

Here is an auction of what I meant. http://cgi.ebay.com/ws/eBayISAPI.dll...853090859&rd=1

They're basically meant for machines that do not have a reversing spindle. They work pretty good as long as you compensate Z correctly for the floating head for blind holes.

We have 2 machines that have the 2100 control. Unfortunately I haven't had the opportunity to run either. One is a Cinncinati 3 spindle 5 axis gantry. The other is a high speed 5 axis VMC.

[ryanduc]

Hi Palafox
Sfm For That Material Is 15. So The Formula Is
3.82 X 15 /.25= 229.the Feed Rate 229/18= 12.7
Use Moly-dee Tapping Fluid & Rigig Tap .thanks

[M_D]

There are some situations where you need to calculate feed rate differently. For one thing, there are several different types of tap holders, which will more or less determine the method. If you have a machine that has a rigid tap function, you do not usually need a floating tap hold holder unless the machine synchronization is not good. Some machines are just better than others in that regard.

In that case, feed the tap at the exact thread pitch, or will put stress on the tap and may break it, especially in hard material and/or deep holes. For example, tapping ¼-20 holes in aluminum you could use 20.0 IPM at 400 RPM, or even 40.0 IPM at 800 RPM. For production, we would program even faster, for 1 of a kind projects we tend to keep it more conservative. You don’t need to make 20 FPM and 400-RPM increments, but I like to keep it even as I don’t like to round off the feed rates.

Some machines are programmed with the pitch for the federate. For example, the feed rate for a 20 threads per inch tap would be F.05 (1 divided by 20 = .05), and for a 32 thread per inch tap it would be F.03125 (1 divided by 32 = .03125).

Some tap holders have tension and compression, some extension, and some only compression. If you don’t have compression, then you want to feed the tap a little slower than the pitch, so the tap is extended for some give at the reversal. If you didn’t have extension, then you might need to feed it a little faster than the pitch. When a tap holder has compression, then it may compress more or less at the start, depending on hold chamfer and how quick the tap “starts”. So you will use some Kentucky windage on both depth and federate at times, to suit the situation, as it can’t be calculated exactly before hand, although with experience your first estimate should be in the ballpark. Even a different RPM may affect when the tap actually starts, and thus the depth.

Also, some stainless steel alloys are much more forgiving than others, 303 is pretty good, where as 304 is noticeably more difficult. We have tapped 100’s of thousands of 6-32 holes through ¼” 303 at 400-800 rpm (depending on the machine) with Trim Sol cutting fluid, with very little tap breakage. But good tap fluid is an extra insurance when you are in doubt. Also, drilling the holes just a little bit larger on difficult jobs may provide plenty of thread strength for the job, but reduce your tapping woes significantly.

[Rekd]

I've always had the best luck using form taps. (Roll taps?) They're a lot stronger, and give stronger threads.

Tap drill diameters are slightly more critical to hold any class threads. A change of only a few thou can change the % of engagement quite a bit.

[M_D]

Roll taps are good, we have used them to tap 1/8" 0-80 holes in 304 where standard taps didn't hold up. The one thing about roll taps I don't like is on through holes it tends to distort the hole at the exit more, essentially forming a burr. A standard tap seems to leave a cleaner hole on the exit side.