compound infeed for threading

[g30u0w0]

Can someone please explain this concept to me as I am stilling learning to thread effectively.
TY,
G30

[cam1]

Hi:
When threading using a 60 degree V tool, the tool can be advanced into the OD by either making moves on just the X axis, or moves in the XZ, which allows just the leading edge of the threading cutter to do the cutting. For deep threads, the quality of the threads is better when using compoubd infeed, as again the leading edge of the 60 degree tool does the cutting. On a manual lathe the compund would be set to 29.5 degress, and infeed would be made using the compound, as opposed to the cross slide (90 degrees to work axis).

regards

[g30u0w0]

Originally Posted by cam1 Hi: When threading using a 60 degree V tool, the tool can be advanced into the OD by either making moves on just the X axis, or moves in the XZ, which allows just the leading edge of the threading cutter to do the cutting. For deep threads, the quality of the threads is better when using compoubd infeed, as again the leading edge of the 60 degree tool does the cutting. On a manual lathe the compund would be set to 29.5 degress, and infeed would be made using the compound, as opposed to the cross slide (90 degrees to work axis). regards

I very much apreciate the help. So when using this coding how do I control the infeed?
G76P030060R0.005Q50
G76X...Z...P...Q80F...
Thank you
G30

[g-codeguy]

Originally Posted by g30u0w0 I very much apreciate the help. So when using this coding how do I control the infeed? G76P030060R0.005Q50 G76X...Z...P...Q80F... Thank you G30

60 is the compound infeed. Remember that the infeed is half of that...30 degrees in this case. I normally won't use 60 unless trying to eliminate chatter. It has the least amount of tool pressure. However, it is only cutting on the leading edge. This means that the trailing edge is rubbing. Generally not a good thing. Especially in work hardening materials, but it does work.

The 03 means you are making 3 spring passes. Not a good thing either for work hardening materials. Sometimes necessary to keep consistent size or remove taper. I prefer to remove taper with an R-value in the 2nd block. Q50 means minimum cuts of .005 per side. Possibly a little heavy. R.005 means the last pass takes .005 per side. See previous comment.

There are 6 options for Fanuc controlled machines. I normally start with 55 or 29. Only used 0 once in almost 23 years.

[g30u0w0]

Originally Posted by g-codeguy 60 is the compound infeed. Remember that the infeed is half of that...30 degrees in this case. I normally won't use 60 unless trying to eliminate chatter. It has the least amount of tool pressure. However, it is only cutting on the leading edge. This means that the trailing edge is rubbing. Generally not a good thing. Especially in work hardening materials, but it does work. The 03 means you are making 3 spring passes. Not a good thing either for work hardening materials. Sometimes necessary to keep consistent size or remove taper. I prefer to remove taper with an R-value in the 2nd block. Q50 means minimum cuts of .005 per side. Possibly a little heavy. R.005 means the last pass takes .005 per side. See previous comment. There are 6 options for Fanuc controlled machines. I normally start with 55 or 29. Only used 0 once in almost 23 years.

The example I posted was for a brass part, but I will remember your advice if running anything harder. If you get a chance can you give an example of when you think it would be a good idea to use29 rather than 55 or 60 rather than ... I guess an application example of each would help. I am in the process of updating most of my thread calls as you suggested. Luckily I did not program many parts before asking the questions : )
Ty again for the post.
Chris

[g-codeguy]

As previously stated, I don't use 60 infeed for any material unless trying to remove chatter. You shouldn't need any spring passes on brass unless running a very small diameter part that is pushing away from the insert. DOC for last pass and minimum passes you had are also fine in brass. The Q80 in your example may be fine...or it may be too light. Depends on thread height. It is fine for something like a 32 pitch thread. If thread height was in the neighborhood of .03, then I would be using Q100 or Q120, maybe more, depending on the number of passes I wanted.

To be honest, I've never noticed much difference between 29 or 55 degree compound infeeds. I must admit that I never tried testing both infeeds on the same job to see if insert life was longer with one or the other.

When running stainless I normally use G76P000055R.003Q30 or G76P000155R.003Q30. The difference being whether or not there is thread relief at the end of the thread. I use 00 if there is relief, and 01 if not. 00 will leave a ring at the end of the thread if there is no relief. 01 pulls out at .1 times pitch. Often I am threading to a shoulder, and need the thread to get very close to the shoulder. Stainless may be a case where 29 would be better than 55 because the trailing edge will be taking more material. My problem is that I am normally running small parts, and chatter becomes a big factor. Usually (but not always!) less tool pressure is better for removing chatter.

Something to remember when trying to get close to a shoulder: Insert grade and pitch may say to thread at S3000. Problem is the higher the spindle speed, the sooner the insert starts withdrawing. You may have to drop below S1500 to get close enough to the shoulder. I've found that going below S900 doesn't make any difference. I have one job that I not only run at S900, but have to grind a notch in the side of the insert to clear a seat. It is the only way the thread can be gotten to the desired depth. Problem with that is the insert is running below its optimum range. Some grades handle it better than others. I have found Sandvik inserts to be one of the best in this situation while Seco inserts can be one of the worst, although Secos are very good when running within their specified range. Another good one is Kennametal KC720 or KC5025, tho Sandvik is better.

The P & Q in the 2nd block can be used for a few different things. One is if the insert is chipping on the first pass. Lie. Make the P larger while keeping the Q the same value. This will give a shallower 1st pass while keeping the number of passes within reason. Making the Q too small can result in way too many passes.

Sorry for the length of my post, but hope it will be of some help to you.

[g30u0w0]

no the post is perfect length. that is exactly the info I need. I am going to cut and paste your post to word for future consulting.
TY,
Chris