Rigid tapping overloading servo

[123tool]

Hello everyone, I've learned alot from this forum but have a problem I can't solve. I tapping a 1/2-13 hole about 1 inch deep in 6061, the bore is 7/16 (oversize) and using a new spiral tap. About 3/4 into the cut the servo kicks out, the tap is packed with chips but I tapped this same part 6 months ago without any problems. I have a TM-1P which has never let me down but this time...

Can I rigid tap half way then finish the hole, if so how would i program this move? Any thoughts or ideas to try tomorrow.

Thanks, Doug

[txcncman]

You should be able to do peck tapping on a machine with rigid tapping. Check your machine manual.

[123tool]

I'll give that a try tomorrow. There are many things to learn, without any formal training it takes a a little longer to figure it out. Matter of fact I bought 2 Haas a couple years ago and didn't know anything except how to push the start button. It's been fun.

Thanks again,
Doug

[underthetire]

May be time to tighten the belt.

[miljnor]

you didn't give any specifics but it could be one of your servo drives going bad.

or if its an old brush machine it could be the servo brushes going bad too.

[123tool]

Thanks, it's a couple years old without much abuse, the guy who did the programing is unable to help due to family issues so I'm on my own. I can't program without OneCNC so to change this will be trial and error.

We have a hobby based business where all the parts are set in fixtures then run, I'll look at the manual today then be back with questions tonight.

Thanks again,
Doug

[KenFoulks]

Turn on setting 133 (Repeat Rigid Tap)

Here is a snippet of example code:
G00 X0 Y0 Z.1 M08
G84 Z-.5 R.1 F10.
G04 P1. (Fill the hole with coolant and flush chips)
G84 Z-1. R.1 F10.

Repeat Rigid Tap will take an additional one second or so for every tapped hole. It will always repeat as long as the part doesn't move and the starting point (R value) is the same for both codes.

[KenFoulks]

One more thing, check your coolant concentration. If there is too much water, tapping (especially in aluminum) becomes very difficult.

[123tool]

Turn on setting 133 (Repeat Rigid Tap)

Here is a snippet of example code:
G00 X0 Y0 Z.1 M08
G84 Z-.5 R.1 F10.
G04 P1. (Fill the hole with coolant and flush chips)
G84 Z-1. R.1 F10.

Repeat Rigid Tap will take an additional one second or so for every tapped hole. It will always repeat as long as the part doesn't move and the starting point (R value) is the same for both codes.

Thanks, I wish I would have seen your post early today it would have saved some time. The hole turned out to be 3 1/2 inches deep with the bottom two inches tapped. The code was the same repeating the G84 a couple of times then added a G80 to clear everything for the next part. This is run on a fixture plate that is generic, it has 5 small vises mounted so we can run smaller batches and save a bit of time.

G84 Z-2.25 F70;
G84 Z-3.0 F70;
G84 Z-3.375 F70; I don't think I need this line
G84 Z-3.75 F70;
G80;

Thanks agin for the help,
Doug

[KenFoulks]

Just as a matter of habit, add decimals to all values. There are settings (77&162) to control how values are interpreted when a value is received without a decimal. If these settings were changed, this may result in a crash.

R values are another example of a default setting. If you put R.2 on the first line and no R value on the second and the default is .1 the result would be a cross-threaded hole. G98 and G99 also have some influence over this behavior.

Lastly, setting 130 (Tap Reverse Multiply Speed) may result in broken taps in some situations. If the value is 2, the tap will pull out of the hole twice as fast.

[djc1965]

Try slowing the rpm and feed down a bit. We used to have a robodrill at where I used to work that would do this or produce a spindle overheat alarm. I assume you are using an rpm of 910 on the spindle. That might be a bit much. Your 6061 Aluminum might not be as clean this time as in the past. I have machined mostly aluminum for more years than I care to admit and have seen the properties vary in both extruded and die cast aluminum which have produced different results when machining including some where taps last long where other times we go through many. I could go into this a lot more but this post would end up being way too long. Try cutting the speed and feed 25% and see if that works, if for any reason just to experiment a bit. I also agree that upping the coolant concentration a bit may help.