Need Help!- How to program thread milling?

[Vegabond]

Hello.

I have now recieved a threadmill from Iscar but i don`t actually know how i use it.

From the reseller i get a code like this.....

G90 G0 G54 G43 G17 H1X0 Y0 Z10 S1320
G0 Z-25
G01 G91 G41 D1X 4.75 Y-4.75 Z0 F41
G03 X4.75 Y4.75 R4.75 Z0.25
G03 X0 Y0 I-9.5 J0 Z2.0
G03 X-4.75 Y4.75 R4.75 Z0.25
G01 G40 X-4.75 Y-4.75 Z0
G90 G0 X0 Y0 Z0
M30
%

Can someone explain these codes for me? i know several, but not all.
And what code do i need to change if i want to mill a bigger diameter, more/less pitch, and so on.....

I don`t understand this text actually...
Look at side C119 http://www.rinos06.ru/doc/ISCAR_rezb_frez.pdf

I run a fadal machine..


Greetings from Robert.

[Geof]

Thread milling is just the same as interpolation with a Z movement included; helical interpolation.

The code you show is for doing an internal thread.

The first line sets the tool on center 10mm above the work. The work zero has to be at the center of the part.
G90 G0 G54 G43 G17 H1X0 Y0 Z10 S1320

This line moves the tool down 25mm for the start of the thread. It will be cutting a righthand thread using G03 (climb milling) so the tool has to 'screw' itself out of the hole.
G0 Z-25

This line changes to incremental and starts tool compensation with a move that only takes the tool halfway to the thread diameter.
G01 G91 G41 D1X 4.75 Y-4.75 Z0 F41

This line does an incremental arc to bring the tool into the cutting position. Notice Z moves up slightly because now the tool is starting the thread. The reason the tool arcs into the cut is to make the entry gradual.
G03 X4.75 Y4.75 R4.75 Z0.25

This line does a full circle to complete the thread. The Z movement is the pitch of the thread.
G03 X0 Y0 I-9.5 J0 Z2.0

This line does another arc to move away from the thread.
G03 X-4.75 Y4.75 R4.75 Z0.25

This line cancels tool compensation.
G01 G40 X-4.75 Y-4.75 Z0

This line takes the tool back to center and lifts it to Z0 in absolute coordinates.
G90 G0 X0 Y0 Z0

For different diameters the X and Y moves would be larger or smaller and the R in the arc would change to match them. Also the I value would change to match.

For different pitches the Z moves would change.

[Vegabond]

Hello agian, and thanks for the explanation.

On the fadal isn`t the G43 like others (radius compensation into a line..), on the fadal is it "G43 Tool Length Compensation Positive" What is that mean?, and is it a code on the fadal to radius comensation into a line?


Thanx.


Robert.

[sinha_nsit]

G43/G44 are for setting Z0 at a desired height with a desired tool. This is needed because every tool may have different lengths. Hence the name: length compensation.

G41/G42 are for invoking radius compensation. The program is written as if the radius of the tool is zero. Since the actual tool will have some radius, and every tool will have different radii, radius compensation is needed. You just need to specify different radius values in the offset table, and call G41/G42 with appropriate offset number (e.g., G41 D10). All the calculations are done by the control.

[Vegabond]

I mill threads with a program like this...

G0 Z-10
G1 F300
G1 X-10
G3 X10 Y0 R10 Z-9.5
G3 X-10 Y0 R10 Z-9
G0 X0 Y0
G0 Z10
(End Program)

But i know i can use a easyer method. with using I and J.....
But how do i program it that way, and what are I and J

I=X ?
J=Y ?

I and J is if i want to move the from my fixture offset?

Can someone explain a little bit how this work?


Greetings from Robert.

[angelw]

Originally Posted by Vegabond I mill threads with a program like this... G0 Z-10 G1 F300 G1 X-10 G3 X10 Y0 R10 Z-9.5 G3 X-10 Y0 R10 Z-9 G0 X0 Y0 G0 Z10 (End Program) But i know i can use a easyer method. with using I and J..... But how do i program it that way, and what are I and J I=X ? J=Y ? I and J is if i want to move the from my fixture offset? Can someone explain a little bit how this work? Greetings from Robert.

I and J are code addresses used in conjunction with G02/G03 (circular interpolation addresses) in the X Y plane, describing the location of the arc center being programmed. In most controls, I and J are incremental values relating to the arc center relative to the start coordinate of the arc. In some controls, I and J indicate the absolute value of the arc center coordinates. I relates to the X axis and J to the Y axis.

Given the I and J values, that are effectively two sides of a triangle constructed between the arc start and center, the control software can calculate the radius of the arc (the hypotenuse of the triangle). Error checking can be performed to determine if the programmed end point is on the theoretically correct arc based on the center location described by the I and J values. In contrast, when using the R address in circular interpolation, the end point can be incorrect (within reason) without and error being generated. In this case, the control calculates the arc center based on the arc start, end coordinates and the R value programmed. Accordingly, incorrect geometry can be programmed without being aware of it. Full circles (360 degrees) can't be programmed using the R address.

Regards,

Bill

[ad64075]

With all due respect to salesmen who try to push their "thread milling software" onto machinists, they really have little clue as to what works consistently and reliably. The salesman's job is to sell tools, not to tell you how to produce a quality thread nor to tell you how to make your tooling hold up the best.

Thread milling is best done from the top down using conventional milling, not from the bottom up using climb milling. All too often there is insufficient clearance for coolant or chip evacuation and the tool is subject to a massive amount of tool pressure. Mr. Iscar doesn't care. He can sell more inserts that way.

Try to follow the example below. Depending on your control, you can likely macro the toolpath very easily, or simply cut and paste for multiple holes:

O0001(1"-8 THREADMILL)
T1M6
G0G90G54X0.Y0.S2400M3
G43H1Z1.
M8
X2.5Y2.5 (POSITION CENTER OF HOLE)
Z.1 (CLEARANCE PLANE)
G1Z0.F100. (FEED TO FACE)
G91G42X.5D1F24. (ACTIVATE INCREMENTAL MODE AND RH COMP)
G2I-.5Z-.125 (HELICAL CUT CLOCKWISE, .125 PITCH)
I-.5Z-.125
I-.5Z-.125
I-.5Z-.125
I-.5Z-.125
I-.5Z-.125
I-.5Z-.125
I-.5Z-.125 (FINAL HELICAL CUT .875 DEEP)
G1G40X-.5 (ESCAPE)
G0G90Z1. (ABSOLUTE MODE, RETURN ABOVE PART)

From this point, you could continue on to another hole or end your program or whatever you wish. It is so simple to program thread milling this way, not to mention accurate and quick.

Good luck!

[angelw]

Originally Posted by ad64075 With all due respect to salesmen who try to push their "thread milling software" onto machinists, they really have little clue as to what works consistently and reliably. The salesman's job is to sell tools, not to tell you how to produce a quality thread nor to tell you how to make your tooling hold up the best. Thread milling is best done from the top down using conventional milling, not from the bottom up using climb milling. All too often there is insufficient clearance for coolant or chip evacuation and the tool is subject to a massive amount of tool pressure. Mr. Iscar doesn't care. He can sell more inserts that way. Try to follow the example below. Depending on your control, you can likely macro the toolpath very easily, or simply cut and paste for multiple holes: O0001(1"-8 THREADMILL) T1M6 G0G90G54X0.Y0.S2400M3 G43H1Z1. M8 X2.5Y2.5 (POSITION CENTER OF HOLE) Z.1 (CLEARANCE PLANE) G1Z0.F100. (FEED TO FACE) G91G42X.5D1F24. (ACTIVATE INCREMENTAL MODE AND RH COMP) G2I-.5Z-.125 (HELICAL CUT CLOCKWISE, .125 PITCH) I-.5Z-.125 I-.5Z-.125 I-.5Z-.125 I-.5Z-.125 I-.5Z-.125 I-.5Z-.125 I-.5Z-.125 (FINAL HELICAL CUT .875 DEEP) G1G40X-.5 (ESCAPE) G0G90Z1. (ABSOLUTE MODE, RETURN ABOVE PART) From this point, you could continue on to another hole or end your program or whatever you wish. It is so simple to program thread milling this way, not to mention accurate and quick. Good luck!

Let me first qualify my comments by stating that I'm not a salesman, nor do I have a vested interest in any tooling company.

Although there are limited situations where threading from the top is more acceptable, but generally speaking I don't agree that this is the best method. Whether, the cutting tool being used is a multi-toothed thread hob or a single toothed insert, when starting from above the hole, effectively all of the machining will be done with one tip, the leading tip in the case of the multi-toothed tool.

In the example given, this single point would have done the same amount of work threading the single hole, as a mult-toothed tool would have done machining eight holes. Threading from the top, using conventional milling, will take eight times longer than a multi-toothed tool starting at the bottom of the hole, and four times as long if a roughing and finishing cut is made using the multi-toothed cutter.

More tool wear and poorer surface finish will be experienced employing conventional milling.

Regards,

Bill

[Geof]

Originally Posted by angelw ......Whether, the cutting tool being used is a multi-toothed thread hob or a single toothed insert, when starting from above the hole, effectively all of the machining will be done with one tip, the leading tip in the case of the multi-toothed tool...... .......More tool wear and poorer surface finish will be experienced employing conventional milling. Regards, Bill

In as nice a manner as possible I disagree.

It is possible to use a multi-tooth cutter for an internal thread by conventional milling simply by starting the cut part way down the hole. Of course to do this you do need to do a "tangential entry" so the cutter enters the work gently.

And in my experience conventional milling gives a better surface finish than climb milling both with single point tools and multi-point tools. I had actually started a thread on this topic but not received much feedback.

http://www.cnczone.com/forums/haas_m...ventional.html

[angelw]

Originally Posted by Geof In as nice a manner as possible I disagree. It is possible to use a multi-tooth cutter for an internal thread by conventional milling simply by starting the cut part way down the hole. Of course to do this you do need to do a "tangential entry" so the cutter enters the work gently. And in my experience conventional milling gives a better surface finish than climb milling both with single point tools and multi-point tools. I had actually started a thread on this topic but not received much feedback.

It was my comprehension from your penultimate post that you advocated milling from the top to avoid the "massive amount of tool pressure" the tool will be subjected to due to starting down the hole and milling out. In fact, by starting part way down a hole, and using climb milling, will result in more pressure than climb milling starting at the same point.

When conventional milling, the chip thickness starts at zero and progressively increases until the cutter exits the cut. This action requires that sufficient pressure must be reached before the cutting edge penetrates the work piece surface. Until that happens, the cutting insert slides across the work surface. This rubbing effect provoked by the chip beginning at minimum thickness results in:
1. greater power consumption,
2. increased heat,
3. an uneven cut surface
4. increased work hardening in susceptible material
5. and reduced tool life of up to 50% compared to climb milling.
There have been many documented tests carried out to establish these facts and have been well accepted for many years.

Regards,

Bill

[sinha_nsit]

Any example where conventional is better than climb milling?

[Superman]

Bugger those 2, they can compare their nut sizes between themselves

Here is a link to a few wizards from SECO -- the threading wizard links are down the RH side