Origin/consistency of chipload recommandations

(Vince) #98

These routers have plenty of power to keep up with mods without issue. Ridgidity is the weak link from the beginning if your main concern is cutting metal.

In my experience and research, if you reach a 0.005 chipload and want more MRR, its better to increase load with axial doc.

1 Like

(Vince) #99

Did I mention I picked up a 60krpm spindle, should be here next week. Btw love the data, is there any way we can see your test rig? I was thinking a vice on rails with strain gauges.

3 Likes

(Phil Thien) #100

But that refers to power consumption without consideration of rigidity?

0 Likes

(Julien Heyman) #101

(don’t mind me, just following up on my latest tests)

With the newfound revelation that I can go 200"/min (facepalm…), and since I wanted to test chiploads for soft plastics, in my case HDPE, I extended the table by another factor of x2 (consistent with my previous finding in HDPE, and data from Winston’s video on machining HDPE on the Nomad)

HDPE Acrylic Soft wood / MDF Hard wood Aluminium
acrylic+100% softwood + 20% hardwood + 100% baseline + 100% baseline
1/16" 0.0024"/0.06mm 0.0012"/0.03mm 0.001"/0.025mm 0.0005"/0.0125mm 0.00025"/0.0063mm half of 1/8" values
1/8" 0.005"/0.12mm 0.0024"/0.06mm 0.002"/0.05mm 0.001"/0.025mm 0.0005"/0.0127mm half of 1/4" values
1/4" 0.01"/0.254mm 0.0048"/0.12 mm 0.004"/0.1mm 0.002"/0.05mm 0.001"/0.0254mm baseline

and got those gorgeous HDPE chips using a 2-flute 1/4" endmill at 5000mm/min and 10.000RPM, i.e. a fat chipload of 0.01" :slight_smile:

Sure, it makes more sense to use an O-flute at half the feedrate, but watching the machine hog HDPE was fun.

[EDIT] I fixed the typos, I obviously meant 0.01", not 0.1". I’m so bad at this Imperial units things, I wish I could use millimeters only and still be understood out here :slight_smile:

8 Likes

Bamboo, HDPE, Fusion360, downcut and O-flute party
(Ummm, not sure, but I’ll try...) #102

Thanks so much for rationalizing/quantifying this whole subject for us non-engineers.

3 Likes

(Gerald Mackelburg) #103

Machine rigidity (torsional stiffness) determines how much machine deflection (positional error) results from a given cutting force, which is plotted in the charts. If cutting force exceeds the capability of the machine, something will slip/break. Here’s one way of measuring that limit. Fortunately(?), luggage scales will suffice for Shapeokos because they are far more limited in force. Applying forces to the ends of endmills and measuring the resulting endmill deflections would help determine acceptable forces in the X, Y, and Z axes.

2 Likes

(Gerald Mackelburg) #104

Looks like this 60kRPM spindle did you get the collets too?
I’ve learned that it’s much easier and accurate to measure spindle cutting power, RPM, and calculate cutting force than it is to measure/calculate it. But, I’d be happy to provide info on both approaches if you like.

1 Like

(Gerald Mackelburg) #105

What depth and width of cut?

0 Likes

(Julien Heyman) #106

DOC was 0.125", stepover was probably the same I would have to double check

2 Likes

(Gerald Mackelburg) #107

The end of Podcast 006 supports the @Vince.Fab claim that 0.001" is a good starting point for chip-load, even in much harder metals. This video explains the value of using greater cut depths (which the lower chip loads enable) and demonstrates the value of using quiet spindles. Or, you could “drink the Kool-Aid” provided in Podcast 007.

0 Likes

(Vince) #108

The Nomad liked 0.002 chipload in titanium…

3 Likes

(Phil Thien) #109

So it seems like a Podcast w/o any video? Is there a link to a video you intended to post?

I listened to about the last 1/4th of program #6, so I can learn about the chipload vs. DOC thing, but I didn’t hear it, can you narrow-down where they go through that please/

TIA!

1 Like

(Julien Heyman) #110

Using what endmill diameter ?
Just asking because I recently applied the recipe from the table discussed above in the thread, to do a profile cut using a 1/8" endmill in aluminium, targeting a chipload of 0.0005" (halving the 0.001" for 1/4"), and it turned out to be too little, so I used +50% feedrate override and the cut went perfectly. So I would tend to update that table with 0.00075" starting value for 1/8" and 0.0015" for 1/4".

1 Like

(Gerald Mackelburg) #111

Blockquote
So it seems like a Podcast w/o any video? Is there a link to a video you intended to post?
I listened to about the last 1/4th of program #6, so I can learn about the chipload vs. DOC thing, but I didn’t hear it, can you narrow-down where they go through that please/
TIA!

No video that I know of as mentioned in the Podcast 001.

OOPS forgot the link to the DOC and sound of cut video - sorry! I’ll add it to the original post.

Starting chip-load mention is about 57 minutes into Podcast 006.

Thanks for making me look up TIA! I’m kind of old I guess.

0 Likes

(Phil Thien) #112

Thanks, I guess I did hear that the first time, the accent may have thrown me off.

And thank you for the link!

0 Likes

(Gerald Mackelburg) #113

@Julien @Vince.Fab @Everyone Else

IMO it would be really helpful and beneficial for folks to provide full details when they post results. IE material being cut, endmill used, depth of cut, width of cut, spindle speed, feed rate, as well as spindle/router and machine used.

3 Likes

(Julien Heyman) #114

agreed, and I actually try to do this whenever I can, this one just happened to be in another thread

3 Likes

(Vince) #115

That’s alot of information to put just to say it liked 0.0015 to 0.002 actual chipload, and that’s spread over facing, adaptive, boring and contour ops. Chatter was addressed usually with feed override. Tool pressure +1

Adaptive on Nomad
5000 rpm, 164sfm, 4 flute 0.125
40ipm, 0.002 chipload, 0.0015 actual maximal chip
Titanium 8mm-0.080"
0.020 Radial Doc, 0.030 axial

2 Likes

(Luc) #116

I would also add the type of Shapeoko or Nomad, if it is equipped with upgrades like HDZ that may impact rigidity as they will all have an impact on F&S.

1 Like

(Gerald Mackelburg) #117

@Vince.Fab
Thanks for the added info. Here’s why I think its useful.
Feed rate (IPM), axial depth of cut (ADC), and radial depth of cut (RDC) are necessary to determine material removal rate (MRR = IPM X ADC X RDC). MRR and material type determine how much cutting power is required. Cutting Power = MRR X material’s unit power. Cutting power (HP) = Cutter Speed (RPM) X Cutter Torque (ft-lbf) / 5252. Cutting force (lbf) = cutter torque / cutter radius. Machine and workpiece force = Cutter force.

3 Likes