Spindle Load vs. Spindle RPM

Which is the true test of how hard your machine is working ?

If you had to watch the spindle speed meter or the spindle load meter on your CNC machine ... lathe or mill ... to determine if your machine was working too hard, which one would you choose?

The truth of the matter is that although the spindle load meter does tell you the power draw on the spindle motor, the RPM gage is a more accurate representation of how hard the spindle is working. Most machines come with a specific rating for load % per a specific time such as (in laymans terms) : "You can run this machine at 100% for 30 minutes."

That is of course a true statement and you can watch the load meter while cutting and reach that spec. However, if you watch the RPM gage while cutting and see it fluctuate wildly - basically because the motor is trying to keep the spindle at the specified (programmed) RPM - you'll never reach that 30 minute time frame. Because the cutting is so heavy in this type of case, the motor must keep "powering up" to keep the programmed RPM specified. This takes much more power draw on the motor than simply running constant at 100% load for the 30 minutes.

The Solution : When your machine is cutting, watch the RPM gage first to insure that the cutting conditions are resulting in a smooth RPM for the spindle and not wild fluctations as the motor fights to keep the speed constant. Secondly, adjust the cutting conditions so that the load meter is as high as you think you want (there is nothing wrong with 70-75%) and then recheck the RPM gauge to make sure that the RPM's are smooth at those settings. Smooth RPM cutting will result in better life for the spindle motor and smoother surface finish on the workpiece as well.

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!

Canned Cycle Drilling and R Plane Tricks

Wasting time drilling air when "drilling" holes in a part with multiple levels is not uncommon for the novice programmer. In this Making Chips post ... we would like to discuss the always important R plane and how you can easily control it in your G code program.

First ... the FACTS :

There are two planes that the programmer needs to be concerned with :

INITIAL PLANE ... this is the plane used for rapiding around the workpiece. This plane should always be set high enough to avoid the workpiece as well as any clamps or other fixture related objects that can be struck by the tool as it moves around the part.

• On  Fanuc controlled or Haas machine ... the initial plane is defined as the last Z position before the canned cycle is called. So in the sample code below :

G00 G90 Z1.000

G98 G81 Z-.500 R.050 F1.0

• Z1.00 would be considered the INITIAL PLANE ... because it is the last Z position prior to the the G81 canned cycle command.
• In an Okuma machine ... the user can set the INITIAL PLANE by commanding a G71 Z--- line prior to the canned cycle command line. So ... imitating the above Fanuc line ... we would program :

G71 Z1.000

G81 Z-.500 R.050 F1.0

R PLANE : The R plane is defined as the plane at which the drilling operation begins. So basically the tool rapids from the Initial Plane to the R plane ... and then starts the drilling operation. The R plane is defined in the canned cycle command line. So in the above examples ... R.050 is defined as the R plane ... the point where the drilling operation would begin.

In the above programs ... the tool would rapid from the Z1.00 initial plane to the Z.050 R plane.

After drilling ... we can tell the tool where to return by using the G98 ( initial plane return ) or G99 ( R plane return ) ... for Fanuc / Haas ... in the canned cycle command line. Once commanded ... G98 / G99 becomes modal ... which means the machine will remember where it is supposed to return ... until told differently. When programming for Okuma ... we can use the M53 ( like G98 ) / M54  ( like G99 ) commands.

NEXT ... the TRICKS :

Did you know that you can very easily change the R plane when drilling on uneven surfaces?

Did you know that you can very easily change the return point between the INITIAL and R planes?

As mentioned above ... once G98 or G99 is set ... the control remembers where to go.

Also ... once the R plane is set in the canned cycle command ... it remembers where the R plane is.

But you can change either very easy ... just command it !! Like this :

(1) G00 G90 Z1.000

(2) G98 G81 Z-.500 R.050 F1.0

(3) X1.00 Y1.00

(4) G99 X2.00 Y2.00

(5) X3.00 Y3.00 R-.100

(6) G98 X4.00 Y4.00 R.050

(7) G80

(1) - Sets the Initial Plane as Z1.00

(2) - Sets the R plane as Z.050 ... return to the Z1.00 after drilling this hole

(3) - Drill this hole ... R plane is .050 and return to Z1.00 ... these were modal from (2)

(4) - After drilling this hole ... return to R plane ... still set to Z.050

(5) - Drill this hole but start at the new R plane of Z-.100 ... return to Z-.100 after drilling ... G99 is modal.

(6) - Drill this hole but start at the new R plane of Z.050 ... return to Z1.00 after drilling this hole G99.

(7) - Cancel the canned cycle ... all modal canned cycle information is cleared.

On an Okuma machine ... users can set and re-set the Initial Plane through the G71 command. On a Fanuc / Haas control ... this is not so easy. You would have to cancel the current canned cycle with a G80 ... move the Z axis to the desired Initial Plane ... then re-command a new canned cycle to set a new Initial Plane.

So ... as we illustrated here ... it's fairly easy to efficiently and effectively machine holes on uneven surfaces using a combination of the return plane commands G98 / G99 / M53 / M54 and R plane settings. Although the Initial Plane. So ... STOP CUTTING AIR !!!

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com
Conversational CAD/CAM
Quoting & Estimating
G Code Conversion
CNC Training
.... and MORE !!!