Different results between G1/2'' and G3/4'' with the same tool

[FBL]

Hi everyone,

I have a part on which I made a 1/2'' internal thread, immediately followed by an operation to make a 3/4'' internal thread, with the same tool.

When it comes out of the machine, I test the threads with "go no-go" gauges in good shape. The 1/2'' thread is good, but not the 3/4'' (too tight, the "go" gauge does not fit).

In the Mastercam program, the diameter of the 1/2'' is set to 20.955, and that of the 3/4'' to 26.441. The diameters of their holes before the two operations are made in helical bores, respectively of diameter 19 and 24.5. They are correct when measured when they come out of the machine, which leads me to believe that it is the thread bottom that is not good.

Note that the 1/2'' is in G17 at the end of the part with an overhang of about 100 mm, and the 3/4'' in G19 just above with the same overhang.

Could someone explain this difference in machining quality, made with the same tool? Is it possible to apply a different tool correction between two operations of the same program for the same tool?

Thanks for your help!

[crazy^millman]

Think about the surface area that is being machined and that should answer your question for you. What is the circumference of the 1/2 thread verses the 3/4 thread? The distance cut by the tool is greater in on than the other but the same exact method and process is used and you are expecting the same exact results? Sorry never going to beat the laws of physics here. Normally when doing this I will have one D offset for the 1/2 and D offset for the 3/4. Then we adjust the offset accordingly to what the size difference comes out to be. I was doing one part where I had 8 different diameters using the same tool years ago. I had 8 different D numbers for each +/-.0002 holes being machined by the tool. On a Mill/Turn with limited live tooling locations and had to make what the customer had purchased work.

[FBL]

Hello crazy^millman,

Indeed, with these differences in circumferences, it may be wise to apply different compensations on the tool depending on the different operations.

I have never worked with different D offsets on the same tool, could someone explain to me how I can set this in the program. I imagine that it depends on the machine used, but I should be able to manage with the basic principle.

I have trouble finding explanations on the internet, but I see that when the tool is called, at the start of the operation, a D offset is associated with it. But I am told that the D number corresponds to the tool slot, and not to a compensation value. In addition, I do not find a D when initializing the programs after generating the code (see attached the start of the G1/2'' thread operation).

Should we add lines of code directly on the machine after generating the code to call the corresponding D offsets?

I am interested if you have screenshots of existing programs, or if you know of tutorials already online on the internet.

Thank you very much for your help,

[crazy^millman]

How are you generating the NC code? Your Cam software should allow you the ability in each operation to define the correct D unless you have a forced D process because of Tool Life management, If this is the case which is does look like since that seems to be Siemens NC code then you will have to discuss this process with the MTB(Machine Tool Builder) to best see what is the correct process to control different D values for that specific machine.

[FBL]

This is a G-code generated via our Mastercam post-processor, made to generate Siemens NC code indeed.

I have never seen a D value generated in our codes yet. We apply G41 and G42 corrections to our tool radius, which allows us to adjust the radius parameters in case of wear.

But this therefore requires setting a single correction value for all operations performed by the tool in question.

I think that in this case I should contact our MTB to discuss this topic and see how we can manage this.

Thanks for the advice

[jstell]

There's a slightly different discussion of this here:

In threadmill you don't have the stock to leave option, but you do have the override geometry option in cut parameters, or draw an arc of the size you need if you are working in a version that predates the addition of that feature.  Then once you know the relation between the two threads compensation, you can just repost.  Of course, it might be simpler to just use two tools if you have room in your magazine/carousal.

[Kyle F]

seems like there are many ways to get around this one.

on our matsuuras we have G10 lines to set H and D wear

" G10 L13 P#517 R.000 ( SET WEAR FOR D ) "  --- (#517 is "whatever tool is in the spindle")

so if I have a threadmill doing a 8-32 and then a 10-32, I'll just place a different tool between the 32TPI toolpaths and I'll get a G10 line output for each thread....

Not sure if that's the 'right' way to do it, but it works LOL. On a non-palletized machine I would probably just lie to one of the toolpaths in the CAM via major thread dia override

[Leon82]

we had an issue where an m1.6 thread in titanium came out tighter in the back thread which was deeper. we just ran with two D offsets. and when we went to high volume we used two tools one for each thread

[Paul Anderson]

here is the start of a program from my Siemens control. I am only knowledgeable on the TNC640 and the new S1 controls. After the tool change, there is a D1 callout. This is for the first instance of the tool. In the tool table you should be able to make multiple instances of the same tool. Each new instance will create a new D value. Notice the D1 after the tool change. Another instance of the same tool will use D2 and so on. Anything previous to the TNC640 I am not sure of.

 

DEF REAL _camtolerance
DEF REAL _X_HOME, _Y_HOME, _Z_HOME, _B_HOME, _C_HOME
;
_X_HOME=0 _Y_HOME=0 _Z_HOME=0
_B_HOME=0 _C_HOME=0
;
G17 G710 G94 G90 G55
_camtolerance=0.02
TRAFOOF
SUPA G0 Z=_Z_HOME D0
SUPA G0 X=_X_HOME Y=_Y_HOME
SUPA G0 B=_B_HOME C=_C_HOME
MSG("MILL_ROUGH")
T="12MM_ROUGH"
M6
D1
CYCLE832(_camtolerance,_ORI_ROUGH,0.8)
G55
ORISON
G0 B=DC(90.) C=DC(180.)
CYCLE800(1,"KIN1",220000,57,0,0,0,0,-90,0,0,0,0,0,0)
G0 X6.5 Y-5.99906 Z77.52 S8090 D1 M3 M8
CYCLE800()
TRAORI
G17 G0 X-77.52 Y-5.99906 A3=-1. B3=0.0 C3=0.0
G0 Z6.5 A3=-1. B3=0.0 C3=0.0
G0 X-64.20635 A3=-1. B3=0.0 C3=0.0