[jorgehrr]

My first time programming a thread mill.

I need to program 5/8-13 thread, I have not clue.

Any samples or web sites that I can learn from will be appreciate.


Thank you

Jorge

[Mitsui Seiki]

http://www.micro100.com/downloads/ThreadMillAssist.html

Take a look at this.It may be of some help to you.

[Geof]

Can you program a circle? For example G03 I0. J-.3125 Fsomething.

This does one counterclockwise circle around a centerpoint located negative 0.3125 on the Y axis. (Actually some controls interpret the J value as the absolute Y coordinate; mine interpret it as the incrmental distance from the location of the tool.)

Can you do helical interpolation using incremental? G91 G03 I0. J-.3125 Z0.0769 Fsomething.

This does one CCW circle but during the circle the tool moves up the distance Z.0769; in other words it has cut one thread.

Thread milling is simply helical interpolation where the Z movement per circle is the thread pitch. To do a right hand thread 3/4" deep you start at the bottom and spiral your way up.

G91 G03 I0. J-0.3125 Z.0769 Fsomething L10

This does ten CCW circles and moves up a total of 0.769"; it has cut your thread.

I have left out all the details about moving to the hole location, moving out to the starting position with tool comp and all that stuff. If you know any G-code you should be able to sort things out from this.

[jorgehrr]

Thank you guys.

This is great information

Jorge

[Bluesman]

Thank you guys.

This is great information

Jorge

I thinbk if you got to the OSG websight they have a program you can download that will generate G code for thread milling. I know that tere catalouge comes with it I would guess you could get for the web sight too

Bluesman

[tobyaxis]

http://www.micro100.com/downloads/ThreadMillAssist.html

Take a look at this.It may be of some help to you.

Hey these are good to have for the future.

Thanks!!!

[mrplace]

[QUOTE=Geof;323187]Can you program a circle? For example G03 I0. J-.3125 Fsomething.

This does one counterclockwise circle around a centerpoint located negative 0.3125 on the Y axis. (Actually some controls interpret the J value as the absolute Y coordinate; mine interpret it as the incrmental distance from the location of the tool.)

Can you do helical interpolation using incremental? G91 G03 I0. J-.3125 Z0.0769 Fsomething.

This does one CCW circle but during the circle the tool moves up the distance Z.0769; in other words it has cut one thread.

Thread milling is simply helical interpolation where the Z movement per circle is the thread pitch. To do a right hand thread 3/4" deep you start at the bottom and spiral your way up.

G91 G03 I0. J-0.3125 Z.0769 Fsomething L10

QUOTE]


I am still pretty new to CNC, so go easy. I do not fully understand I, J and K. Is I the same as X and J the same as Y, except they are circular movements? If not, how do I determine my I and J coordinates?

This is how I have learned to make a circle.

G2 X.5 Y.25 R.25 F10
G2 X0 Y.25 R.25

This makes a circle, but makes it very hard to make threads since you are just cutting two 180's. I have downloaded the spreadsheet and Advent's program, but I would like to have a grasp on the actual mechanics of the code.

Thanks for any assistance.

http://www.advent-threadmill.com/2_downloads.cfm

[Geof]

I am still pretty new to CNC, so go easy. I do not fully understand I, J and K. Is I the same as X and J the same as Y, except they are circular movements? If not, how do I determine my I and J coordinates?

This is how I have learned to make a circle.

G2 X.5 Y.25 R.25 F10
G2 X0 Y.25 R.25

This makes a circle, but makes it very hard to make threads since you are just cutting two 180's. I have downloaded the spreadsheet and Advent's program, but I would like to have a grasp on the actual mechanics of the code.

Thanks for any assistance.

http://www.advent-threadmill.com/2_downloads.cfm

I have seen this and have started preparing a reply but got distracted. As the advertisements sometime say: 'Watch this space' to quote a famous military figure... I will return.

[Geof]

I am still pretty new to CNC, so go easy. I do not fully understand I, J and K. Is I the same as X and J the same as Y, except they are circular movements? If not, how do I determine my I and J coordinates?

This is how I have learned to make a circle.

G2 X.5 Y.25 R.25 F10
G2 X0 Y.25 R.25

This makes a circle, but makes it very hard to make threads since you are just cutting two 180's.

Okay, going easy (I hope).

I, J and K, where did I mention K? Are you trying to confuse me?

Getting serious:

All the following is correct for Haas machines.

Circular interpolation moves; the G02 clockwise motion and G03 counterclockwise motion, for a partial circle can be programmed using the Radius method or the I, J method but for a full circle it is necessary to use the I, J, method.

You can understand why the R method does not work for a full circle when you look at what the G02 or G03 command is telling the machine to do with the R method.

In absolute programming G02 says follow a clockwise circular path with a radius equal to R from your present position to the position X, Y.

In incremental programming G02 says follow a clockwise circular path with a radius R from your present position to a position located a distance X and a distance Y from your present position.

G03 just says follow the counterclockwise path.

For a full circle the start position and end position are the same, or looked at it another way the distance travelled is zero. So using the R method for a full circle means you are telling the machine to go to the position it is already at in absolute or telling it to go nowhere in incremental.

It is possible to do almost a full circle using the R method. In fact when you tell the machine to move on a circular path between two points you always have two choices; the short way in which the circle covers less than 180 degrees or the long way which covers more than 180 degrees. Giving R a negative value tells the machine to go the long way round.

Of course it is possible to do two half circles using the R method to get one full circle; or any combination of two partial circles. For a full circle in one command the I, J method has to be used

With the I, J method the effect of the G02 or G03 command is slightly modified; G02 says move in a clockwise circle all the way around to your starting point using the position defined by I and J as your center point. G03 is move counterclockwise.

In this command the center is located the distance I along the X axis from the starting point and the distance J along the Y axis from the starting point.

As an example imagine the Work Coordinate is located at the center of a 1.000" dia. hole that has to be interpolated. Using a 0.500" dia cutter the centerline of the cutter has to follow a radius of 0.250".

If the tool is positioned first at the Work Zero, X0. Y0. a move to Y0.25 puts the cutter at the correct radius; the distance back to the center point is 0.250". The circular interpolation command for counterclockwise motion is:

G03 I0. J-0.25

The J is negative because the Y move was positive; if the Y move was negative the J would be positive.

I is 0. because there was no X movement from the center point to the starting point for the circle.

When using the I, J method for full circles absolute and incremental has the same effect; the circular interpolation command says follow a circular path back to this point using the point defined by I and J as your center point.

Because the command returns to the same point no incremental motion has occured; because the command returns to the same point it has returned in absolute to its original location.

Thread milling makes use of this by using incremental to command an incremental Z move during the circular interpolation.

To end I will comment that it is possible to use R for thread milling and it is possible to do partial circles with I and J but not tonight .

[mrplace]

OK, that makes alot more sense to me now.

You didn't mention K, it is in something I am reading and states it is also a circular motion.

Thank you for the detailed explantion.

[Kool Parts]

This is for single point tool that I have.
Gary

%
O0
G17 G40 G80 G90
(3/8 THREAD MILL 5/8-13 TPI)
T2 M6
S6500 M3
G0 G90 G54 X0.0637 Y0
G43 Z1. H2 M8
G0 Z0.1
G1 Z-1.0269 F10.1
G41 X0.0625 D2
G3 X0.126 Z-1. I0.0318 J0
Z-0.9231 I-0.126 J0
Z-0.8462 I-0.126 J0
Z-0.7692 I-0.126 J0
Z-0.6923 I-0.126 J0
Z-0.6154 I-0.126 J0
Z-0.5385 I-0.126 J0
Z-0.4615 I-0.126 J0
Z-0.3846 I-0.126 J0
Z-0.3077 I-0.126 J0
Z-0.2308 I-0.126 J0
Z-0.1538 I-0.126 J0
Z-0.0769 I-0.126 J0
Z0 I-0.126 J0
X0.0625 Z0.0269 I-0.0317 J0
G1 G40 X0.0637
G0 Z0.1
Z1.
G0 G49 G90 Z0 M9
G28 G91 Y0 Z0
M30
%

[Geof]

OK, that makes alot more sense to me now.

You didn't mention K, it is in something I am reading and states it is also a circular motion.

Thank you for the detailed explantion.

There are machine related differences which is why I mentioned my info is correct for Haas.

I just realised maybe K is when you are working in a vertical plane; doing circular motion in X and Z or Y and Z, K would be the distance to center along the Z axis. This is motion in G18 and G19.

[jorgehrr]

Geof.
Thank you for your explanation in how to make circles, now....
How do I relate this information to accomplish my thread mill.

Please if possible an example will be great.
Again...thank you for sharing your time with the rookies.

Jorge

[Geof]

Geof.
Thank you for your explanation in how to make circles, now....
How do I relate this information to accomplish my thread mill.

Please if possible an example will be great.
Again...thank you for sharing your time with the rookies.

Jorge

If you re-read my explanation in Post #3 after reading the stuff about circles in Post #9 you should be well on the way to getting it straight, or seeing that we are talking about threads maybe I should say you should be starting to getting really screwed up .

Very bad puns aside, have a look at Kool Parts program:

You will see how he has the G3 command which takes the tool down to Z-1. then on each subsequent line the tooling is 'screwing itself' out of the hole.

As a side comment I should mention that you do not need to keep repeating the G3 command; it stays in effect until you program something different.

On the line immediately following the G3 during the circle motion the tool moves from Z-1. to Z-0.9231 and this is a distance of 0.0769" which is the pitch of a 13tpi thread.

Each circle moves up by this same amount which is why I say the tool screws itself out of the hole...making the thread as it goes.

In Post #3 I described doing it in a different manner. Because the G3 command works the same in both Absolute and Incremental you can do all Kool Parts' circles in a single line with an Incremental command:

G91 G3 I-0.126 J0. Z0.0769 L12

Screws the tool out of the hole in exactly the same manner.

Kool Parts probably generated his code using a computer; I am computer incompetent so I have to do it the hard way and like to economise on typing.

There are other things in Kool Parts' example like Tool Compensation and what looks like a lead-in circle which need a longer explanation; I need to go and do some work to justify my existence. If you want something longer ask I I will see what I can generate this evening or over the next few days.

[Kool Parts]

Yes, just used Surfcam to generate program for Haas post. If I had to know how to do it and explain like Geof did my brain would explode:drowning:

Hole is X0. Y0. And is for the correct size hole. I like to thread mill from the bottom up and I used a 1 inch deep hole. The tool is .373 dia in the tool registry as experience with that tool has shown.
I also forced a D so I can adjust the tread fit to suit in a test piece.
Gary

[Geof]

Yes, just used Surfcam to generate program for Haas post. If I had to know how to do it and explain like Geof did my brain would explode:drowning: ....

What makes you think mine hasn't , or feels like it might.

[tobyaxis]

What makes you think mine hasn't , or feels like it might.

I did some thinking about a few things this afternoon at work. The more that we use PC applications for Programming CNC's the more we forget the manual programming.

Progress is starting to look more like stepping backwards. Goef your explanation is great an reminded me of the days before CAD/CAM.

Programming Manually teaches a lot while Programming with Software allows you to forget.

[Geof]

I did some thinking about a few things this afternoon at work. The more that we use PC applications for Programming CNC's the more we forget the manual programming.

Progress is starting to look more like stepping backwards. Goef your explanation is great an reminded me of the days before CAD/CAM.

Programming Manually teaches a lot while Programming with Software allows you to forget.

Careful now! First dangerous move is thinking at work you might draw attention to yourself.

Second dangerous move is that you seem to be expressing some thoughts getting awful close to my views on the topic of CAM and manual programming. You are likely to get all the attacks I have experienced trying to convince me I am a stick-in-the-mud-fuddy-duddy-backward-Luddite who obviously does not have the smarts to compete in this modern computer dependent world.

[tobyaxis]

Careful now! First dangerous move is thinking at work you might draw attention to yourself.

Second dangerous move is that you seem to be expressing some thoughts getting awful close to my views on the topic of CAM and manual programming. You are likely to get all the attacks I have experienced trying to convince me I am a stick-in-the-mud-fuddy-duddy-backward-Luddite who obviously does not have the smarts to compete in this modern computer dependent world.

Yea, and when that PC crashes and you don't have one with CAD/CAM??????

I believe that I am becoming too dependent on my PC for even simple tasks. This is bad

[drewmeister]

here are several excel "programs" that make circular hole boring, helix boring and thread milling very easy. just input a couple of variables and you are good to go!