[Karl_T]

A lot of my machining involves drill and tapping. I've had a need to able to put a tap in a collet and rigid tap for some time. This should work in theory as Galil supports electronic gearing. But there is no mention of this ability for a mill without a servo spindle in the Camsoft manuals. I have a 2J type head on a CNC knee mill. The spindle is run by a VFD.

Getting rigid tapping to work turned out to be an epic struggle. At one point the great<Camsoft> technical help implied that it might not be possible to do this on a machine without a servo drive spindle. Today, I'm here to say that doing the difficult with Camsoft is routine. Impossible just takes a little longer.


After I got G84 working, I spent another day and improved all the other canned cycles as well. I made an effort to comment the heck out of the code so that most any programmer can follow the logic. I'm sure the macros will take some minor mods to run on another machine.

Attached is the code for all canned cycles. Enjoy


Karl

[Karl_T]

I came back to rigid tapping a few weeks ago and had trouble. Find Index (galil FI) quit working reliably, don't know why. I also had troulbe with resetting registers again. Do a search and replace as outlined below. The macro worked with these changes for the last couple weeks.







IF \864=0 THEN COMMAND DP,,,,0:COMMAND GA ,,E :COMMAND GR ,,\860
'if first time through;FindIndex mark,set spindle to slave Z,electronic gear ratio

'NOTE changed to DP,,,,0 on 04 05 09 program bugging on FI


...clipped main program....



COMMAND GR ,,0 'turn off electronic gearing
'MACHDISP
'MACHHOME3 \868 'current home readout
'MACHZERO ;;\868 'rezero to current home readout
'ABSDISP
'NOTE: Above 4 lines needed because registers get confused with electronic gearing

SLEEP 1.0
READOUT3 \869 'current Z position
HOMEZ \869
'NOTE first four lines above bugging 04 10 09, second trial

[Ox1]

Have almost got the kit ordered, but it just dawned on me that I have not heard much of the rigid tapping option.

I read these posts recently, and ass u me that all is well, but you never said what it was exactly that you used instead of the servo motor I don't think?

I ass u me'd that you found a way to mount an encoder off the actual spindle somehow?

A servo motor shouldn't really be what is needed exactly is it? I have a resolver that is set originally for spindle orient that I am planning on upgrading, and I would like to think that CamSoft can work with that eh? I would think it to be perfect, but the words "Rigid Tap" only pull up 5 threads total, and only this one is titled as related. 2 of the others are locked! (Those may be worth investigating?)

(Turns out they are 5 to 6 yrs old and I am sure that some things have changed since then eh?)

I am more interested in hearing from someone that "is tapping" or maybe more importantly "Aint Tapping" then someone saying that it can be done. But I would appreciate any comments. :stickpoke


---------------

Think Snow Eh!
Ox

[Al_The_Man]

No 1, you need an encoder driven off the final spindle shaft.
If you take a look at commercial systems like Mitsubishi and Fanuc etc, they use tight control of the spindle, although the drive is basically a AC Vector rated motor & VFD, the system usually has a pulse generator or encoder of some kind on the motor back to the VFD for accurate control of the motor, as well as the encoder on the final shaft to gear the Z axis to.
I have found so far that the Galil gearing feature works well, you would need to confirm with Camsoft as to how well it works with their system.
You may have a problem integrating a resolver with Galil however.
Al..

[Karl_T]

I read these posts recently, and ass u me that all is well, but you never said what it was exactly that you used instead of the servo motor I don't think?

I ass u me'd that you found a way to mount an encoder off the actual spindle somehow?
...
Ox

Encoder is mounted on the spindle shaft, a resolver won't work. The spindle motor is three phase with VFD. And a good DC brake.

I've tapped a few thousand holes. Werks grate!

Karl

[Ox1]

As I said - the orient resolver is scheduled to be "upgraded".


Karl = 'nother screen name on 'nother site. :idea:



----------------------

Think Snow Eh!
Ox

[Ox1]

Did a gander at your macro and I see that you were using your back geared setup in the equassion and that _ that was the issue at hand.

My setup has the encoder 1/1 with the spindle so it should be elementary....


... but as is noted on G84 - it denotes "NON-rigid tapping".

Not "Rigid".

Will the canned G84 doo rigid as is? And if so - why doo they call it "NON"?


Also - I have a 3 speed geared head and I fully expect it should tap in any gear as the encoder is on the spindle shaft it'self. (Or driven off of enyways...)



------------


Think Snow Eh!
Ox

[Karl_T]

Did a gander at your macro ...


Think Snow Eh!
Ox

You're WAY ahead being able to go right on the spindle. makes life much easier. Yes, this custom macro is for rigid tapping only. I'm not sure where you're reading about NON-rigid tapping but it does not apply.

I'm glad to see somebody using this work. Let me know when the chips are curling

Karl

[Ox1]

I'm glad to see somebody using this work.

Well - As I read it - your saying that I don't need to use your werk eh?



-------------

Think Snow Eh!
Ox

[miran70]

OK i was wondering how can i program a jump height into the drilling cycles i need a p plane programmed into the cycles because of clamps and different sized parts i cant seem to get this to work for me and its a serious problem thanks ahead of time for any help.
mike

[camsoft]

The G84 canned cycle like most of the other canned cycles has a R word for Rapid Clearance plane where the value after the R is the Z height to jump to clear clamps or fixtures.


Tech Support
CamSoft Corp.
[email protected]
PH 951-674-8100
Fax 951-674-3110
PC Based CNC Control For The Machine Tool CNC Retrofit And CNC Controller OEM Market

[miran70]

ya but if you put in say R5.0 it will start feeding from that point im talking about whats called a P plane as in any other controllers it will be listed as say
G00 Z5.000 G81 Z-.300 R.1 F1.5 P1 X0.0 Y0.0 P1 is a jump height of 5 inches between holes rapid plane remains at .1
as of now the only way i see to do it is to create a new drill cycle for each hole

[camsoft]

You can have both R and P in a G81 or G84.

We can tell you that any of the canned cycles are fully user customizable.

Both R and P can be given on the same line.

We would not recommend the G00 Z5.000 on the same line as G81. Place this on the line before G81. If a rapid and Z position such as G00 Z5.000 will always be given then the R does not need to be given in the canned cycle.

It's hard to give a specific advice because we don't know what software product or version you have. You can do this yourself if you are familar with our commands. Most other systems have fixed canned cycles but in CamSoft the canned cycle logic and order of events is user definable. If you don't know how you can contact your dealer to make this happen.


Tech Support
CamSoft Corp.
[email protected]
PH 951-674-8100
Fax 951-674-3110
PC Based CNC Control For The Machine Tool CNC Retrofit And CNC Controller OEM Market

[miran70]

yes i know the G00 Z5.00 goes in the line before the G81 cycle it is what sets the P plane Ive tried putting the P in the same line as the r plane and depth and such it doesn't seem to read it i guess ill have to take a look at the logic to see if i can get it to work boss wont hire anyone to fix this.

[Karl_T]

ya but if you put in say R5.0 it will start feeding from that point im talking about whats called a P plane as in any other controllers it will be listed as say
G00 Z5.000 G81 Z-.300 R.1 F1.5 P1 X0.0 Y0.0 P1 is a jump height of 5 inches between holes rapid plane remains at .1
as of now the only way i see to do it is to create a new drill cycle for each hole

Well, you can program anything you want in Camsoft. The way I did my canned cycles: Look at the current Z position for the rapid traverse plane. ie. if you want rapid taverse at Z=5 just do a G0 Z5 first. Then the R plane is the height to start drilling. Nearly always 0 as i set Z0 as the part top surface.

G0 Z5
G81 X1 Y1 Z-2 R0 F4

will rapid at z=5 to x=1 y=1, then rapid to Z=0 then feed at 4ipm to z=-2

There is no reason you can't program the P value to be the upper plane if you'd rather.

[miran70]

Mmmm it does that for one hole but what if you have 20 holes will it go back to 5 inches away then do it again? mine isn't im wondering if someone didn't finish the logic or something

[Karl_T]

Yes, goes back to Z5 at end of each hole. Just add the X Y coords after the G81, its modal.

Early in this thread is the example code for all the G8x canned cycles.

Karl