Heidenhain -can you increase the spindle RPM in a program without a tool cal?

D

Dan B

Hot Rolled

Joined

Feb 18, 2006

Location

Ontario, Canada

• Feb 1, 2018

• #1

We are attempting to write a wash program using a spindle mounted fan. The fan is supposed to start at 2000 RPM and then ramp up to 8000 RPM maximum. However, if I put a higher spindle speed in with a tool call (to the same tool) the spindle stops for a half second before starting up again. That defeats the purpose of ramping up the RPM. Is there a way in Heidenhain code to add a higher spindle RPM without the spindle briefly stopping?

Thanks,

Dan

 

F

FK

Aluminum

Joined

Mar 13, 2007

Location

WISCONSIN usa

• Feb 1, 2018

• #2

Short answer; yes, it can be done.

Longer answer; without knowing the machinie, spindle, drive, ETC. I'm going to guess the pause you are seeing is the spindle changing gears for a different range. Or, rather than gears, a different winding for different RPM range. That last bit might not be worded correctly but its about like that. I'm a machinist, not an electrical Eng.

Try a different jump, like 1000 to 2000 and see if there is a dwell. You might find that 0 to 8000 RPM is the same "gear" and 8000 an up is another. So going from 1000 to 7000 would be no pause.

 

G

gustafson

Diamond

Joined

Sep 4, 2002

Location

People's Republic

• Feb 1, 2018

• #3

Yeah, I don't think it is the control, my DMG has a pause at a certain speed[it escapes me where, mebbee 5k] as mentioned above.

 

S

swarf_rat

Titanium

Joined

Feb 24, 2004

Location

Napa, CA

• Feb 1, 2018

• #4

I was under the impression that what exactly happens at a tool call is MTB dependent. On an HH control, you can execute a tool call with only speed as a parameter, no tool number, feed, etc. On a well written PLC, this should just change the spindle speed and nothing else. On a poorly written PLC, any tool call may do a number of things like stop and start the spindle.

TOOL CALL S8000

should just change the spindle speed to 8000 rpm. If you have feed, tool numbers, axis etc in there, its more likely that the PLC dealing with the tool call will stop the spindle. Of course a well written PLC will stop the spindle to change gears, if that is required.

 

D

Dan B

Hot Rolled

Joined

Feb 18, 2006

Location

Ontario, Canada

• Feb 1, 2018

• #5

Thanks for the responses. It's a Hermle so I'm guessing it's a well written PLC. :-)

I've also discovered since asking this question, that you can ramp up the RPM with variables.

I'm going to try the TOOL CALL S8000 as it is a simple solution, but if that doesn't work I will play with the variables.

2 Q10 = 50 ; Tool Number
3 L X+0 Y+0 R0 F5000 M92
4 L C+0 A+0 R0 F5000 M126 M92
5 TOOL CALL Q10 Z
6 Q1 = 1000 ;Spindle Speed
7 LBL 1
8 TOOL CALL Q10 Z SQ1
9 L M3
10 L Z-150 R0 F5000 M92
11 L Z+0 A+30 R0 F5000 M92
12 L X+399 A+0 R0 M92
13 L X+0 Y-750 C+180 R0 M92
14 L X-350 Y+0 C+0 R0 M92
15 L X+0 A-30 R0 M92
16 Q1 = Q1 + 1000
17 CALL LBL 1 REP15 ; Sub Reps

 

F

FK

Aluminum

Joined

Mar 13, 2007

Location

WISCONSIN usa

• Feb 1, 2018

• #6

Hermle, yes, spindle winding issue. Like a high and low. After a certain RPM, it changes how power is delivered to the motor. Like at 6000 or 8000.

So, from 2000 to 4000, no pause. 5999 to 6000 (or what ever) pause.

 

D

Dan B

Hot Rolled

Joined

Feb 18, 2006

Location

Ontario, Canada

• Feb 1, 2018

• #7

You are correct. 6000 RPM.

Thanks,

Dan

 

B

bryan_machine

Diamond

Joined

Jun 16, 2006

Location

Near Seattle

• Feb 1, 2018

• #8

I think you want line 8 to be TOOL CALL Q1 rather than Q10

 

D

Dan B

Hot Rolled

Joined

Feb 18, 2006

Location

Ontario, Canada

• Feb 2, 2018

• #9

Q10 is defined as 50. That's the tool number. Q1 is the speed.

It doesn't matter anyway, because even stepping up the RPM in this manner has the spindle stop when it hits 6000.

For now we are maxing the fan at 5999 RPM, but we're going to go with a solid fan that can start above 6000 RPM.

Thanks,

Dan