How to determine spindle speed on Makita RT0701C router

Accessories
1

The router has numerical speed settings, my tools call for a spindle speed of 18,000 rpm. Does anyone know how to determine how the numerical settings relate to actual spindle speed?

1 Like
2

It’s in the manual and also has been discussed many times on this forum.

5 Likes
3

Hey Gerald, hey Nick,

I have this little pic of it:

Maktia_RT0701C__Speed_Adjusting_Dial
Maktia_RT0701C__Speed_Adjusting_Dial368×691 28.7 KB

Source: Makita RT0701C trim router’s Instruction Manual

7 Likes
4

I tested mine with a tachometer and it agreed with the table, within reason. If you are concerned you can buy your own tachometer. Mine has reflective tape you put on the router nut, and it counts the number of revolutions per minute. Very simple, not very pricey. I think I got it from Amazon.

1 Like
5

Thanks very much, I never thought to look in the manual. My mistake, at any rate, I really appreciate the reply.

Kind regards,
Jerry

6

That’s really great information. Not too terribly concerned, but after researching it a little, it became apparent that it’s not an even progression, by that I mean, the spindle speed at 3 is not half of what it is at 6. I’m about a week old at CNC routing and I’m trying to follow the speeds suggested by the Amana tool library specs.

7

It looks very linear between settings 2 and 5 (which is backed up by Jake’s tachometer data posted on these forums).

Thanks to everyone (Andy, Jake, Aiph5u) for this important info.

1 Like
8

I am going to modify my Fusion360 post processor to tell me which dial to set the router too.
Here is the simple formula,

X is RPM speed
Y is Makita Router Setting
Y = 0.000231X−1.0338

Probably also want to round the result to the nearest 0.5.

image
image752×452 9.32 KB

Might have to go polynomial, but I think for simplicity and starters this works.

Though as @Festdewalkita pointed out, if you drop the first and last values (unlikely values to be used anyway), it’s very linear.

Y = 0.0002X - 0.4

image

Here is the post processor modification,

Find this line,

writeBlock(
            sOutput.format(spindleSpeed), mFormat.format(tool.clockwise ? 3 : 4)
        );

Replace with,

writeBlock(
            sOutput.format(spindleSpeed),
            mFormat.format(tool.clockwise ? 3 : 4),
            mFormat.format(0),
            formatComment("MSG, Spindle speed " + spindleSpeed + " RPM, Set Dial to " + ((0.0002*spindleSpeed) - 0.4))
        );

You will then get messages like this,
image

9

That’s pretty cool.

Right now I add the router speed setting to the description in my tool setup in VCarve. Then I include that in the toolpath name so when I load the toolpath it’s telling me the bit & the router setting. More manual than a speed controlled spindle but it’s working for me so far. :slight_smile:

10

Alex, the line in “Replace with” is identical to the line replaced!
Did you forget something or am I just not seeing it?

11

Hey Chris,

you got to scroll code line horizontally :slight_smile:

1 Like
12

Ok Alex thanks.
I do like this addition also.

1 Like
13

Alex, I just used this addition to my Fusion 360 post and it does popup up the messagebox but the program keeps running. It does not stop and give me time to change the dial.
Is there a way to put a pause in it?

14

When the popup shows up, that is your time to change the dial.
When the popup is displayed the program is effectively paused.

15

Well in my CNC code it does not pause. It shows the popup but at the same time continues on and plunges into the work. The first time i had to lunge for the stop button.
Here is the pertinent part of the code:

(2D ADAPTIVE1)
(T1)
N25 S14000 M3 (MSG, SPINDLE SPEED 14000 RPM, SET DIAL TO 2.4000000000000004)
N30 G54
N35 G0 X0.7075 Y0.7526
N40 G43 Z1.45 H1
N45 G1 Z0.95 F100
N50 Z0.85

16

Hmm, interesting.
Mine looks like this,

N30 S18000 M3 (MSG, SPINDLE SPEED 18000 RPM, SET DIAL TO 3.2)
N35 G54 M0 (MSG, WCS change, shift work tile to 1 position.)

So perhaps my next statement containing M0 is what is pausing the run for me and not you.
M0 is an unconditional PAUSE
You can achieve the same with this modification,

writeBlock(
            sOutput.format(spindleSpeed),
            mFormat.format(tool.clockwise ? 3 : 4),
            mFormat.format(0),
            formatComment("MSG, Spindle speed " + spindleSpeed + " RPM, Set Dial to " + ((0.0002*spindleSpeed) - 0.4))
        );

This will result in for you,

N25 S14000 M3 M0 (MSG, SPINDLE SPEED 14000 RPM, SET DIAL TO 2.4000000000000004)

Thanks for pointing this out!

1 Like
17

Alex, That worked perfectly.

Thanks for this, I think it is a definite improvement for those of us using the Makita router.

1 Like