CNC Rethreading????

I know this forum has a lot of Very smart Machinest... I am presented with a problem that Hopfully someone has solved. We are running production parts on a CNC with a internal thread.. The way the loading system is set up we could get up to 5 Parts with Bad Threads before discovering it.. How would anyone suggest rerunning these tools to pick up on the start lead of thread to repair these other than throwing them in the garbage.. Material is semi hard 45rc so taping does not work well.

There has to be some way to locate and remachine? Im probably missing something and thats why I turn to you. (Threadmill? Single Pt? Tap? Beaver with sharp teeth? )

Regards,

Index before turning if possible or economical? Are there ops before this one?

Its a real problem.
What i have done as part of a training job was to write a single threading line with G33.
It was short and just above actually cutting.
I could see where I was in relation to the thread center.
Then I moved my Z start point over a little and moved my X depth in a little and run again.
Do this, its pretty fast and once you have it lined up, use a G76 cycle.
If you need it, a G76 example is on my website doccnc.com.
Good luck: Heinz.

turningcrazy said:

I know this forum has a lot of Very smart Machinest... I am presented with a problem that Hopfully someone has solved. We are running production parts on a CNC with a internal thread.. The way the loading system is set up we could get up to 5 Parts with Bad Threads before discovering it.. How would anyone suggest rerunning these tools to pick up on the start lead of thread to repair these other than throwing them in the garbage.. Material is semi hard 45rc so taping does not work well.

There has to be some way to locate and remachine? Im probably missing something and thats why I turn to you. (Threadmill? Single Pt? Tap? Beaver with sharp teeth? )

Regards,

Click to expand...

Irrespective of the threading cycle used, the big issue is locating the part so that the threading tool tracks precisely in the existing thread groove. You don't mention the control involved, but there are some that have a feature whereby the threading tool can be manually positioned in the thread with the spindle stopped, and a Thread Restart Sequence executed.

In the absence of such a feature, one method that is remarkably accurate in getting the threading tool to track in the existing threading groove is as follows. This method is quite quick and convenient with an external thread. Its a little more difficult with an internal thread, but doable. The smaller the thread diameter, for an internal thread, the more difficult it becomes.

1. Write a test threading cycle to take just one pass at a diameter slightly smaller diameter than the Minor Diameter (Internal Thread) of your thread, so the existing thread is not damaged during this setup stage.

2. When merely looking at the thread with the spindle running, the Thread appears as a blur. However, if you have your eyes follow the Threading tool as it advances along the Thread, you will see the Thread Groove very clearly. So clear will you see it, that you will be able to determine in which direction, plus or minus, the tool needs to move to have it track correctly and roughly how far out of position in Z the tool is.

3. Once you have determined the direction the tool needs to be moved, guess the amount the tool will have to move in Z, and edit the Z start position of the Threading Tool in the direction and by the amount guessed.

4. Repeat the above until you see that the tool is tracking accurately in the Thread groove.

5. If the Threading Cycle being used is one where the tool cuts in along the angle of the thread, for example, the G76 cycle with a Fanuc control, then the Test Cycle needs to be set so that:
i. the X value is the actual Major Diameter (Internal Thread).
ii. the depth of the first pass is equal to the thread height.
iii. the Wear Offset is adjusted so that the tool tracks at a diameter just smaller than the Minor diameter of the Thread.
iv. carry out the steps 2,3, and 4 to determine the correct Z start position for the tool.

Doing the above in point 5 will ensure that the Threading Tool is in the centre of the Thread Groove when the tool is at full depth.

6. Once you're happy that the tool is tracking correctly, further test this by running the actual threading cycle with its multiple passes, and the Wear Offset reset so that the tool will engage with the Thread when near full depth. By colouring the Thread with marking blue, or a felt tipped pen, you will see quite accurately if the tool's Z start position needs further adjustment.

7. Mark an Index mark on the face of the soft jaw, or whatever the work holding device is, and a corresponding mark on the part that is referenced to the start of the Thread of the part currently in the machine and to which the Threading tool has been adjusted.

8. So that all the above steps don't have to be carried out of each of the parts having to be re-threaded, mark an Index mark on each of the parts, referenced to the start of the Thread.

9. When positioning the part in the Work Holding device, line up the Index mark made earlier on the part and the Work Holding device.

The above may seem somewhat tedious, but in reality, it doesn't take long and is quite accurate.

Regards,

Bill

move the thread to its own op, check each one in the chuck before removal.

I do it all the time thread a piece look where the lead starts say the edge of jaw 1 put the part back in the chuck with the lead in the same place re thread done.

Ya I was thinking if the chuck is at Zero than why couldn't you see where the thread starts and put a mark on the chuck and line them up.. Good to hear that works...

WILLEO6709 said:

move the thread to its own op, check each one in the chuck before removal.

Click to expand...

The time it takes to gauge while still in the chuck is going to be less than the rework. Make the gauging part of the process before it comes out of the chuck.

Assuming this is a Turning center, load a piece of the appropriate threaded stock (mandrel) in one of the turret tool locations. Screw "bad" part onto mandrel and feed it into a known "Z" location. Tighten chucking device and proceed to pick up the first part using one of the above mentioned meathods. All the others will merely be a load and cycle operation.
You should also consider a carbide tap held in a tailstock on the manual lathe. Make sure the tailstock is floating and feed the tap in under power.
Merry Christmass

One thing that I've gotten to work in the past, and I know this is a little weird. Use a Manual lathe, put the part in the chuck, with the part not rotating position a single point threaded in the valley of the thread, lock the gearing into place, and rotate the chuck head by hand to cut what you need. Its slow and difficult, but it works if done right.

Have you tried tapping it? I tap a lot of hardox parts that are right around 45HRC and its way easier than you would guess :-)

If these parts only take minutes to run from blank to finish it may be cheaper to chunk them and fix the issues that caused this.
Unless these are automated cells, there should be no reason not to check threads before it is set on the done table by the operator.
If they are automated I would look at tool life to see how consistent it runs and then look at the tool change intervals to avoid bad parts and smooth running.

If they are expensive you can tap 45 hardness with not much issue since most of the thread has been cut.
If the threads are less than 3/4'' it is gonna be a major bitch to line up on plus if it has a blind shoulder you run a real good risk of crashing your tool into shoulder if you Z- to much.

A manual lathe could handle this with no issue and a lot less chance of a ruined tool holder or part.

Thanks to all.. This is an automated cell and we can not check parts unless we stop the machine. I am liking the Tap Idea,, I think this would be fast and easy. as long and we cut the thread instead of rubbing it with a tap. Floating system in a Mill with a manual chuck. Load part- bring tap down- let it cut and retract.. pitch is critical, Hope we dont have issues.

You can actually do it a lot easier using fanuc controls. I think a haas can also rethread using this method. What you do is just write these following commands together as one process at the very beginning of your program(I used G92 but I think it works for 76 also): 1st line: G00 X15.00 Z20.0, 2nd line: M19 T (whatever tool you thread with), and then M01(turn option stop on when you start the program). Ok what that's gonna do is orientate the spindle to a specific degree. Be sure not to move the spindle after it does this. Your threading tool will activate and then you'll hit the M01. Once the machine stops put it in jog and manually fall in lead with the threads without moving the part. Use like the 2nd or 3rd thread. On I'd threads you'll need a flashlight. Once you've done that go to your G54 offset and press Z0 then Measure. If you're losing a little off the connection put that amount negative into G54 and measure. Now when you lose a little you have to lose in increments of one thread so divide 1 by your threads per inch and make sure whatever you lose is either that number or a multiple of that number. Once G54 is set it'll pick up the threads perfectly. You can take option stop off and run the remaining program uninterrupted. On the first part you'll have to adjust the Z starting point to get the thread to line up(so back off a lot in your x wear offset for the threading tool). But every part you cut with that program from then on will fall in lead perfect with just setting G54 with the thread bar.

Why are you getting bad parts to begin with ? There is no excuse for it.

It is an expensive process.
How much are the parts worth, don't throw good money after bad and some will not make it.
Why is the key question.
Why is there not enough time, money or equipment to do it right but there is time, money and equipment to do it over?
Fixing stuff is fine but you need to make sure that you do not fix it over and over. Band-aids are always profit killers.
If you continually fix things that your production will not hold management starts to expect it as normal.
We the willing - Google Search
You will get tired of pulling a rabbit out of the hat and employees will start to think not so good parts are ok.
Bob

T-Bone420 said:

You can actually do it a lot easier using fanuc controls. I think a haas can also rethread using this method. What you do is just write these following commands together as one process at the very beginning of your program(I used G92 but I think it works for 76 also): 1st line: G00 X15.00 Z20.0, 2nd line: M19 T (whatever tool you thread with), and then M01(turn option stop on when you start the program). Ok what that's gonna do is orientate the spindle to a specific degree. Be sure not to move the spindle after it does this. Your threading tool will activate and then you'll hit the M01. Once the machine stops put it in jog and manually fall in lead with the threads without moving the part. Use like the 2nd or 3rd thread. On I'd threads you'll need a flashlight. Once you've done that go to your G54 offset and press Z0 then Measure. If you're losing a little off the connection put that amount negative into G54 and measure. Now when you lose a little you have to lose in increments of one thread so divide 1 by your threads per inch and make sure whatever you lose is either that number or a multiple of that number. Once G54 is set it'll pick up the threads perfectly. You can take option stop off and run the remaining program uninterrupted. On the first part you'll have to adjust the Z starting point to get the thread to line up(so back off a lot in your x wear offset for the threading tool). But every part you cut with that program from then on will fall in lead perfect with just setting G54 with the thread bar.

Click to expand...

I'm betting the OP has long since sorted this matter by now?

I'm not sure I'm following what's going on here? My machine has a "Thread Repair Function" I've yet to set it up but in the instructions you do do a measure after aligning the tool with the thread. Not understanding why your doing a "Z0 measure" resetting G54 Z0 inside the thread?

Brent

yardbird said:

I'm betting the OP has long since sorted this matter by now?

Brent

Click to expand...

So, I have been following this thread for 3 and half years waiting for the right answer. Duh just set Z zero inside the already threaded part!!! Why didn't I think of that?

R

one thing you could do if you have room in the turret is add another threading tool. Figure out how many parts does it run until the threads start going out of tolerance. Say if its 30 parts average, set up a sub program to run 25 parts, then have it run another sub to run the next 25 with the next tool. If you have the room you can set up as many bars you need.