Hi Guys,

Im working on getting my machine to do rigid tapping. Looks like i have to use an M code and my own C programming to do this right? This is going to be difficult to get working with cam software. I really dont want to have to edit Gcode every time i post it out. Would be great if i could use the standard G84 format.

Tom is there any way you could set this up so G84 works like all the other canned cycles but when it gets in position above the hole, it would execute my own C program and when finished move on to the next hole and repeat? Would be awesome if you could set this up somehow. 

Is G84 supported now at all? If it is im assuming you program IPM with floating holder and hope for the best right? Thanks in advance.

Mark

Hi Mark,

I can't think of a simple way to do that with out adding a lot of options.  I suppose tapping in other planes should also be considered.

Below is an extract from rs274ngc.cpp which is what the current code does (basically what you describe).

Here is a description of how it might be implemented currently using an MCode:

http://dynomotion.com/Help/Mach3Plugin/Mach3RigidTapping.htm

Regards

TK

/* convert_cycle_g84

Returned Value: int
   If the spindle is not turning clockwise, this returns
     NCE_SPINDLE_NOT_TURNING_CLOCKWISE_IN_G84.
   Otherwise, it returns RS274NGC_OK.

Side effects: See below

Called by:
   convert_cycle_xy
   convert_cycle_yz
   convert_cycle_zx

For the XY plane, this implements the following RS274/NGC cycle,
which is right-hand tapping:
1. Start speed-feed synchronization.
2. Move the z-axis only at the current feed rate to the specified bottom_z.
3. Stop the spindle.
4. Start the spindle counterclockwise.
5. Retract the z-axis at current feed rate to clear_z.
6. If speed-feed synch was not on before the cycle started, stop it.
7. Stop the spindle.
8. Start the spindle clockwise.

CYCLE_MACRO has positioned the tool at (x, y, r, a, b, c) when this starts.
The direction argument must be clockwise.

For the XZ and YZ planes, this makes analogous motions.

*/

static int convert_cycle_g84(    /* ARGUMENTS */
    CANON_PLANE plane,        /* selected plane */
    double x,            /* x-value where cycle is executed */
    double y,            /* y-value where cycle is executed */
    double clear_z,        /* z-value of clearance plane */
    double bottom_z,        /* value of z at bottom of cycle */
    CANON_DIRECTION direction,    /* direction spindle turning at outset */
    CANON_SPEED_FEED_MODE mode)
{                /* the speed-feed mode at outset */
    static char name[] = "convert_cycle_g84";

    CHK((direction != CANON_CLOCKWISE),
    NCE_SPINDLE_NOT_TURNING_CLOCKWISE_IN_G84);
    START_SPEED_FEED_SYNCH();
    cycle_feed(plane, x, y, bottom_z);
    STOP_SPINDLE_TURNING();
    START_SPINDLE_COUNTERCLOCKWISE();
    cycle_feed(plane, x, y, clear_z);
    if (mode != CANON_SYNCHED)
    STOP_SPEED_FEED_SYNCH();
    STOP_SPINDLE_TURNING();
    START_SPINDLE_CLOCKWISE();

    return RS274NGC_OK;
}

 

Hi Guys,

Im working on getting my machine to do rigid tapping. Looks like i have to use an M code and my own C programming to do this right? This is going to be difficult to get working with cam software. I really dont want to have to edit Gcode every time i post it out. Would be great if i could use the standard G84 format.

Tom is there any way you could set this up so G84 works like all the other canned cycles but when it gets in position above the hole, it would execute my own C program and when finished move on to the next hole and repeat? Would be awesome if you could set this up somehow. 

Is G84 supported now at all? If it is im assuming you program IPM with floating holder and hope for the best right? Thanks in advance.

Mark

On 2017-04-07 18:21, mmurray70@... [DynoMotion] wrote:
> Yes maybe we could use G84.1 or something like that. I see some
> machines use this for ridgid tapping.
>
> Have you given this any further thought Tom? Is there any way you can
> setup a custom canned cycle where it positions to top of each hole and
> runs our C program? This might be very handy for other things as well,
> not just tapping.
>
> I have my rigid tap program working on my machine. But its going to be
> a real pain if i have to manually write code for every hole. Thanks.
>
> Mark
>
>
> Links:
> ------
> [1]
> https://groups.yahoo.com/neo/groups/DynoMotion/conversations/messages/14572;_ylc=X3oDMTJyaGtoNDFqBF9TAzk3MzU5NzE0BGdycElkAzE1ODU4MDAxBGdycHNwSWQDMTcwNjU1NDIwNQRtc2dJZAMxNDU3MgRzZWMDZnRyBHNsawNycGx5BHN0aW1lAzE0OTE2MTQ0ODk-?act=reply&messageNum=14572
> [2]
> https://groups.yahoo.com/neo/groups/DynoMotion/conversations/newtopic;_ylc=X3oDMTJmNWpvNzlzBF9TAzk3MzU5NzE0BGdycElkAzE1ODU4MDAxBGdycHNwSWQDMTcwNjU1NDIwNQRzZWMDZnRyBHNsawNudHBjBHN0aW1lAzE0OTE2MTQ0ODk-
> [3]
> https://groups.yahoo.com/neo/groups/DynoMotion/conversations/topics/14564;_ylc=X3oDMTM3dHFxYnN2BF9TAzk3MzU5NzE0BGdycElkAzE1ODU4MDAxBGdycHNwSWQDMTcwNjU1NDIwNQRtc2dJZAMxNDU3MgRzZWMDZnRyBHNsawN2dHBjBHN0aW1lAzE0OTE2MTQ0ODkEdHBjSWQDMTQ1NjQ-
> [4] https://yho.com/1wwmgg
> [5]
> https://groups.yahoo.com/neo/groups/DynoMotion/info;_ylc=X3oDMTJmbHBqY2pmBF9TAzk3MzU5NzE0BGdycElkAzE1ODU4MDAxBGdycHNwSWQDMTcwNjU1NDIwNQRzZWMDdnRsBHNsawN2Z2hwBHN0aW1lAzE0OTE2MTQ0ODk-
> [6]
> https://groups.yahoo.com/neo;_ylc=X3oDMTJlN2kwdDZjBF9TAzk3NDc2NTkwBGdycElkAzE1ODU4MDAxBGdycHNwSWQDMTcwNjU1NDIwNQRzZWMDZnRyBHNsawNnZnAEc3RpbWUDMTQ5MTYxNDQ4OQ--
> [7] https://info.yahoo.com/privacy/us/yahoo/groups/details.html
> [8] https://info.yahoo.com/legal/us/yahoo/utos/terms/

TapM119.c-14574.txt

Hi Mark,

There is a Patch ready for testing.  See the wiki here for info:

http://www.dynomotion.com/wiki/index.php?title=Rigid_Tapping_G84_Setup_and_Use

Hopefully there is enough information to allow you to interface to your C Program.

Please check it out and let me know of any questions or issues or changes that you think should be made.

Regards

TK

 

Hi Tom, 

Yes i think that would be great! If you didnt want to mess things up for any existing users, G84.1 would be fine too, either will work for me. 

The standard fanuc style would be for example N010 G98 G84 Z-1. R.1 Q.1 F.0625, It would be nice to have all these numbers downloaded to persist.UserData variables. Dont forget Q so we can add the option of peck tapping which is very handy.

I attached my rigid tapping c program. I modified a few things from Thomas Zamirskis program and also the mach3 example. My spindle is not setup as an axis, just turns on CW and CCW with two bits. I modded the program to work with this rather then change my entire machine which is complicated due to high/low range and orientating speeds etc. I added a delay to the end of cycle to allow the spindle to stop before it stops slaving Z, it ended with a Z axis jolt before. And I also added code to record and print minimum depth reached to help tune overshoot compensator. This could also be used to get a depth perfect on a particular job if you still have a little variation. 

Did some testing with this program today and it works fairly well. I tapped a piece of aluminum flatbar dangling outside a vice so it could flex up and down and measured about 0.005" movement with an indicator while tapping at 800 RPM. Taping a hole in a solid workpiece also worked great. No noticeable difference in pitch diameter ridgid tapping at 200 RPM vs floating. At 800 rpm there was a tiny bit of wiggle with a tap in the finished hole, maybe a thou or 2 bigger but it looks great and perfectly usable for my needs. Testing was done with 1/4-20 tap. 

Let me know when you make the changes Tom and ill adjust program to include R plane variable and anything else that needs to be done. Thanks again!

Mark

 

Opps.  That's a typo.  Just changed to V4.34h.  Please use that Version.

TK

 

Looks good Tom thanks. I will try to get this working tomorrow night.

The wiki site says this is for 4.33, will the patch work for 4.34f?

 

Hi Tom,

I updated to 4.34h tonight and applied the patches and it is reading the proper G84 code from my cam software and executing the test program fine. Looks like this will work perfect. 

Couple minor issues though. First one is the retract variable is not right. Its displaying the value for the clearance or initial plane instead of retract plane which is what we really need. 

Second issue is when moving to another hole after finishing first hole. When its done a hole right now, It moves X/Y/Z all the same time to the clearance height above the next hole. It needs to move Z to clearance plane first and then move X/Y to position. Thanks again.

Mark

Hi Mark,

I'm confused :)

What is G98/G99 supposed to do?  According to:

http://www.cnctrainingcentre.com/news/rigid-tapping-g84-canned-cycle/

it says: depending on G98/G99 it will return to Z3 or R1 before moving to the next position.

For the example GCode:

G0 X1 Y1 Z2
G99 G84 Z-1. R.1 Q.1 F.0625

and the Z parameters passed are:

Bottom = -1.000000
Retract = 2.000000
Peck = 0.100000

Right now the parameter called "Retract" is either 2 or 0.1 depending on G98/G99.  I was assuming the tap would finish at that height.

But now if I understand correctly: You want to always have the Retract value of 0.1 always passed regardless of G98/G99.  And the M code will always finish with Z at 0.1.   Then the PC should decide based on G89/G99 whether to after the Tap rapid to Z=2 or remain at Z=0.1

Is that correct?

Regards

TK

 

Sorry I may have read your post wrong, its late lol. If you were asking about the retract variable problem, I just need to have whatever R value is in the G84 line transferred to a variable. 

Whether your use G98 or G99, the tool is going to end up in the same place when M119 is executed. But we need to know R value since the total distance the machine needs to tap is Z value plus the retract height which is where the machine starts from. 

In your test program below of course the machine actually needs to move negative 1.1 to reach bottom. 

G98 G84 Z-1. R.1 Q.1 F.0625

Hi Mark,

The Patch has been updated.  Please see if it works properly now.

Regards

TK

 

Hi Tom,

Yes G98 vs G99 had to do with which plane it returns to before moving to the next hole. But in both cases it would still rapid to the R plane and then execute tap cycle from the same start point. So yes, for the Tapping C program we just want the R value of 0.1 (for this example) for both G98 and G99. 

The video you did last fall about peck drilling is a perfect example of G98 vs G99. See it here: https://www.youtube.com/watch?v=rnzRSWcLMJ8

I have this working now with G84 on my machine, just need this changed as depths are way off obviously since its adding the wrong R value. Thanks again.

Mark

 

Hi Mark,

Opps.  Please try it again.

Also there should now be a Green Feed Line to the GViewer to represent the Tap Motion.

Thanks

TK

 

Hi Tom,

I just tried it again. The R value thing is working good now. Thanks.

The motion between holes still isnt right. Right now it taps the first hole, retracts vertically as its supposed to and moves to second hole perfectly and taps that hole perfectly, but when its done the second hole, it returns to the first hole in XYZ (on an angle again) and then moves to third hole and taps it. When done third hole it returns to second hole position and then finally finishes the program. Seems like its remembering and returning to the previous X/Y locations the same way it remembers and returns to the Z clearance plane. Thanks. 

Mark

Hi Mark,

Hmmm.  That actually makes sense.  The first line has the Q value specified so we assume we should do Peck tapping the other lines don't so we assume we should not do Peck tapping.

How are we to know to do Peck Tapping or not?

If we pass the last value of Q it might be from some other operation a month ago.

I suppose on the first occurrence of G84 after any other motion command we could set Q=0 if unspecified and then use the last Q value in subsequent G84 calls.

Regards

TK

 

Hi Tom,

I tried the latest patch and its working properly for both G98 and G99. Thanks!

I found one more minor issue. I have peck tapping working now on my machine, but it only works on the first hole. When it does the second hole the value for the Peck variable is Zero. Not sure what could be causing this as all the other variables im using are fine for all holes. Any idea on that? 

Mark

Hi Mark,

Updated patch.  Please try it again.

Thanks

TK

 

Hi Tom,

Thats not the way its supposed to work. Standard fanuc format would be to have Q specified once in the G84 line and the value applies to all holes in the cycle.

Yes i think if you set Q=0 if unspecified and use the last Q value for subsequent G84 calls that should do the trick. Thanks. 

Mark

 

RigidTapCycle M119.c-14651.txt

Hi Dan,

 

Tom,
A few months back we were talking about rigid tapping and I brought up the need to block out any feedrate override and spindle override while rigid tapping. Have you put any more thought to that need and how to execute it?

This should actually be part of any tapping cycle, not just rigid tapping.

-Dan