downcut on plywood = fuzz

[houndel]

Thanks Brian, I gave your settings a try and the results were much better.



This (bottom left) was at 3000mm/min, 16,200 RPM (my spindle control was set at 270hz) 1.5mm stepdown, and 1mm pocket allowance cleaned up on the final pass.

The Z belt is definitely jumping teeth: the pocket to the right of this one was the same settings with 2mm stepdown. The 6mm pocket in CAM is only 2mm deep in wood!

The belt is as tight as I can get it. The aluminium tensioner is as low as it can be and the Z stepper mounted as high as possible. The belt is stamped with 520mm on it, not the earlier larger type. It does feel tight, but clearly is not tight enough. Any suggestions?

Thanks again, I'm really making progress on this with all the help.

[DRobs86]

I agree that 24k was probably too fast but I was trying to get him as close as I could to my proven settings, and I am stuck at 30k.

I disagree with many shallow fast fed passes. Slow the feed a bit to keep the forces acceptable, but put that bit in the stock. Millimeter and sub millineter stepdowns in wood are silly to me. You use the same tiny piece of the endmill to do all the work over and again.

I also think that a 1.5kW spindle is more than capable of some fast fed and deep cuts if thw machine can handle it.

For the record I use one .125 inch endmills and I have never broken one cutting despite probably 6 months of nearly daily cutting with these settings. I use .5 inch flute lengths and put it in the collet probably .05 inch from the flutes. I have even on rare occasion run 13mm deep in mdf at about 1200mm a min.

I am by no means an expert, but thats my two cents.

[WillAdams]

As I noted in the linked post from the wiki I had to use a small pay bar to get adequate tension on the z-axis

[Brian Stone]

I disagree with many shallow fast fed passes. Slow the feed a bit to keep the forces acceptable, but put that bit in the stock. Millimeter and sub millineter stepdowns in wood are silly to me. You use the same tiny piece of the endmill to do all the work over and again.

If you do 10mm step downs, then you only use the same 10mm piece of the end mill every time, so what's the difference if you only use 1mm step downs? You're almost never going use the entire end mill except during finishing passes in contour operations. There is practically no difference between doing many passes versus a few as long as you engage the wood efficiently in either case. The main reason for choosing a particular step down is to adjust the amount of force it takes to engage the wood ~~ Less wood takes less force to engage.

By the way, I'm only talking about roughing passes here, and that was my assumption in the previous post. Finishing passes are a different discussion. There are lots of times where you want to use the entire bit to get a super clean edge on a contour to eliminate ridge marks left by multiple passes. But for roughing, and pocketing, or any case where a lot of material needs to be removed, then multiple passes are almost always ideal.

This is the order of logic that i use for just about every job:
1) Select the chip load (mm per flute per revolution)
2) Select the RPM (typically between 16000 and 20000 for me)
3) Calculate your feed rate: (Feed Rate) = (Chip Load) * (RPM) * (Number of Flutes)
4) Adjust your step down to prevent deflection and bit breakage.

I adjust the step down based on my experience with the particular wood that I'm working with. Soft woods like Hemlock cut really easily at 1 or 2mm step down with high feed rates. Harder woods, like a domestic Cherry that I'm using right now, I'm happier with 0.5mm step down at 3500mm/min, and it cuts as clean as butter. You do have to have reasonable expectations for the Shapeoko. It's not a super rigid machine, and the 1/8" bits that we use aren't super strong. You can't put a lot of force on either of them.

I am by no means an expert, but thats my two cents.

Neither am I, and I think the vast majority of us aren't. If you find one, please bring them here!

[DRobs86]

I understand the point that you are getting at, but lets look at it this way. Suppose your small depth cut is indeed better for longevity of the engaging portion of the flutes given a particular linear footage (I grant that it probably is). I engaged my cutting surface one time. You engaged it 6 or 12 times to complete the same profile operation. My settings have to be 6 to 12 times more inefficient than yours for my endmill to wear out faster than yours. Not to mention, with my setting Ive finished my operation and moves onto the next one.

But hey, I could be wrong. I am definitely bucking convention here.

[houndel]

... Just checked the z belt tension with the app "tension2go" and I am getting 175hz or 39N. Pressing with my finger on the longer side of the belt, I can move it approx a maximum of 8mm. Like Will, I used the pointy end of a file to lever the stepper motor as high as possible before tightening it. Is this as tight as it can get?

How do others fare with plunging depth? I would love to try deeper cuts for comparison, but can't get past plunging 1.5mm at this stage.

[DRobs86]

I dont have an SO but I have built one with a belt driven Z in a luff tackle configuration (so a lot of back and forth on idlers. It seemed to matter somewhat where Z was in its travel when I tensioned it.

How long is the span where you can push it 8mm? Its just too loose I believe.

[WillAdams]

Please don't use a file as a lever --- the temper on them is (or at least should be) too hard, and they're brittle and all-too likely to break. (though this brings up a separate discussion of what the out-sourcing Nicholson is trying to pass off as files these days --- I've exhausted the N.O.S. of the local hardware stores, and haven't turned up any more when travelling lately, so I despair of what I'm going to be doing for files when my current stock is used up)

[TDA]

Thought I'd try to flesh out some of the reasoning for shallow vs deep passes.

The main issue from a tool life perspective is that if you can't maintain a good chip load then you will effect tool life. Let's take the example you gave of 1300mm per minute at 30K RPM. Assuming you are using a standard 2 flute cutter then your chip load per flute comes out to 0.022mm. One of the few ways a cutter can get rid of heat is by dumping it into the material removed by the cutter. So when your chip is so small there is very little material to remove heat. Too much heat and you will wear the tool out much faster. This is also a big reason why you see plastics melting and wood burning at low feeds.

Now let's move on to rubbing. This basically means that the size of the chip you are taking is too small to get the edge of the tool "under" the material you are cutting (CNCCookbook has some good information on this Link). This does more than just adding more heat as it forces the material under the cutting flute and your tool has to push through the material instead of cutting.

Those are two of the basic reasons people will get better tool life with the shallower cut. Even though the tip of your tool is getting several times more use you aren't overheating the tool or rubbing.

Additional to tool life you also have to take into consideration the issue of tool and machine deflection. For those that don't know deflection is basically the tool being "bent" from it's programmed path due to cutting forces. This is an issue both at the programmed feed and every time you come to a stop or make a significant change in direction. When at feed the tool will deflect out of it's programmed path. When the tool stops or changes direction it will "relax" back into the programmed path. As such deflection should be kept to a minimum as it will change the size or accuracy of your finished part. You can reduce deflection by reducing your cut depth, feed, or increase your RPM. However, you have to balance those with the issues above.

Hope that at least gives a little more insight.

[DRobs86]

TDA,

I appreciate the discussion. I agree that things aren't ideal with my settings, but I submit that the kind of machines we are using just force into work arounds.

See this chipload recommendation chart:



For reference, my chipload is 0.00085" (the standard equivalent to what you showed). For hardwoods, the chipload recommended for a 0.125" end mill shows 0.003 to 0.005. This leaves me with about 3.5 times less chipload than the low end of that recommendation. I could instead make 2mm deep cuts, run 3900 mm/min (153 IPM) and get a chipload of about 0.0026, which is much closer to what is recommended. I'd use the same portion of the flute 3 times though. I also feel like you leave more opportunity for these to go wrong (steps lost resulting in misaligned layers, etc) for each pass you make.

At the end of the day though.... we are arguing tool life on a 4 dollar endmill. I concede my settings aren't ideal textbook, but I think I pick up some benefits in doing so.