spindle power / feed rate

Talk about all things CNC
Post Reply
Posts: 60
Joined: Tue Mar 18, 2014 12:10 pm
Location: Jamaica

spindle power / feed rate

Post by noproblem » Wed May 07, 2014 11:55 pm

OK, over the lasr 2 weeks since I have completed my shapeoko 2 I have only been using MDF to cut and mill things .However over the weekend I decided to get more adventurous and start to use new types of wood . So I went to the local hardware and pick a truck full of different type woodS( by the way they gave it to me for free)

Since I was not sure the hardness of these woods I decided to change the normal feed rate from 60 in/min to 30 which I used on the MDF . after doing a simple test cut I notice that the Y axis was struggling to cut when moving in a + or - direction, this + and - direction was against the wood grain. The X axis was fine since it was cutting in the same direction on the wood grain. To fix the Y axis from struggling i lowered the feed rate to 10 in/min which was much better, however there was still little struggling on the Y axis but hardly noticeable.

Now here is my question

Since i am using a 400w Chinese spindle which runs at 12,000 rpm with a two flute straight 1/8 bit .

Do you suggest
1) update the spindle
2) change the bit
3) work with the slow feed rate

Posts: 8628
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15

Re: spindle power / feed rate

Post by WillAdams » Thu May 08, 2014 12:27 am

A spindle which can turn faster would probably be better suited for wood --- pretty much all of the speed data we have on the materials page for wood: http://www.shapeoko.com/wiki/index.php/Materials#Wood_2

is for very high spindle speeds, typically a Dewalt DW660 @ 30,000 r.p.m.

FSWizard does allow one to plug in any desired speed (the default is 10,000 r.p.m.) and includes calculations for mahogany though: http://zero-divide.net/index.php?page=f ... _id=663574
Shapeoko 3XL #0006 w/ Carbide Compact Router w/0.125″ and ¼″ Carbide 3D precision collets

Posts: 4442
Joined: Thu Jul 19, 2012 6:50 pm
Location: Camberley, UK

Re: spindle power / feed rate

Post by cvoinescu » Thu May 08, 2014 12:48 am

Most types of wood do not pose any chip clearance problem, so you could switch to a four-flute endmill to double your feed rate at the same RPM. However, as Will said, a higher RPM would be the even more useful. And there's nothing that says you can't do both.
Proud owner of ShapeOko #709, eShapeOko #0, and of store.amberspyglass.co.uk

Posts: 1351
Joined: Tue Jan 29, 2013 4:51 pm
Location: Minneapolis, MN

Re: spindle power / feed rate

Post by twforeman » Thu May 08, 2014 2:04 am

You don't state what depth of cut you were taking, but I run a 1/4" two flute router bit at 60 IPM through hard maple at a depth of .060" per pass. I am using a Ridgid trim router spinning at around 20k RPM though.
Ender 3 3D Printer
ShapeOko v3 serial #0004 - upgrade thread
All of my ShapeOko related blog posts

Posts: 332
Joined: Wed Mar 13, 2013 5:53 pm
Location: Colorado

Re: spindle power / feed rate

Post by danimal » Thu May 08, 2014 2:44 am

If you have flex about your x axis (moving in the y direction) the torque force applied causes a deflection that tips the end mill further into the material at an angle. This causes all kinds of problems like chattering, bogging down and even deviating off course. The mills are made to cut at a very perpendicular path to the material, so if they are being dragged or driven through the material at an angle they will over load a non-cutting edge, even with a more powerful router. Squaring and increasing rigidity of the carriage and router would be where I would start. Then it is a matter of calculating your feed rate for a given end mill and balancing that feed rate with your pass depth. Your pass depth is limited by the rigidity of your machine.
Shapeoko # 1458

RT0701C Spindle || dual y motor || x axis nema23 with custom carriage 1000mm length || z axis nema23 linear rail upgrade with 1/2-10 ACME

Posts: 60
Joined: Tue Mar 18, 2014 12:10 pm
Location: Jamaica

Re: spindle power / feed rate

Post by noproblem » Thu May 08, 2014 3:09 am

This is excellent

I hear chattering and even deviating off course sometime i guess Out of Sqaure is maybe my issue.

So while writing this post i decided to double check with a level ( thats all i have) i guess what the grantry was off by about 2 - 3 mm tilting foward , so i pulled the all m5 bolts on the grantry plates and now its as straight as the level. The actual Y axis makerslidle was level just the gantry was off.

Will try tomorrow to see if this fixed the problem


Simon P
Posts: 28
Joined: Wed Mar 12, 2014 9:17 pm
Location: Wiltshire, UK

Re: spindle power / feed rate

Post by Simon P » Thu May 08, 2014 12:06 pm

Finally got my shapeoko back up and running! First thing I did was cut new mounts for a Dewalt out of 15mm HDPE. I mention this because this was the first time I'd ever cut anything at all and the following process helped in gauging appropriate speed and feeds for the HDPE and can be applied to any new material.

I used the Zig Zag 'sweet spot' test described on the precisebits website to determine appropriate feed and speeds. They have an equation that relates bit diameter, chip load (they have suggested values), number of flutes and RPM of your spindle to a best guess feed rate. Which you then use as the first feed rate in incrementally faster zigs and zags. The test worked out really well for me although I could only guess the RPM of the dremel since it gets bogged down quickly under load. I was quite easily able to pick out an appropriate maximum feed rate for the conditions. I did the calculation manually and used a combination of makercam and hand coding to create the g-code for the test. Should be easy enough to whip up a script to generate the test g-code in future.

I will note that I do not follow their advice of plunging to a depth equal to the bit diameter. The dremel I was using did not have enough power to do that in HDPE and would stall so I decided to use a plunge depth of half the bit diameter for my tests. I think the main thing is that you use a consistent plunge depth based on bit diameter so that you eventually create a database of comparable test results. You might feel that the calculated feeds seem quite fast but this is a test designed to push the envelope for a particular material, tool and spindle speed. In actual use they state you should only feed at 75% of whatever rate you found best in this test. This is what I did with my HDPE and it worked out perfectly. I intend to follow the same process for any new material and bit combination.

EDIT: Forgot to mention, I also increased the acceleration in GRBL to the 510mm/s/s they suggest. So that the tool was moving at my chosen feed rate more often than not. The default 25mm/s/s means that the tool will rarely reach your chosen feed rate for shorter cuts.
Shapeoko 2 #3697 - Dewalt D26200 Spindle, Precisebits Collets, 250mm Z-Axis Makerslide

Post Reply