Poor Surface at LOW Chipload as well as Perhaps Deflection?

[verhoevc]

Hey guys, I did some searching and couldn't seem to find answers here. My two current issues seem to be:
1- Lower-than-expected surface quality at less than half bit's recommended chipload
2- Poor match-up when milling shapes; half thickness done from the front, flipped, and then the other half of the thickness milled from the back.

Problem 1 details:
Awhile back when first learning feeds and speeds I did the recommended tests with my machine, desired bits, and usual materials. Using a 1/4" single-flute Onsrud upcut O bit (if I read correctly that's a recommendation of .005-.007 chipload in hardwood) I ran channels at various chiploads across hardwood end grain to determine what chipload I should actually use. I found that my best surfaces were .002 and below! The difference between .002 and lower was minimal, so I've been running things at .002. However, even at feeds/speeds using this chipload I'm still finding lower-than-expected surface quality, especially on end grain!
Basically I'm running at .002 (24IPM/12,000RPM x 1 flute) and running .2" DOC climb as a profile cut offset .015" til I reach about 7/8" depth. I then come back and do an onionskin pass full depth to remove that last .015" as conventional. On end grain sections of these profiles I'm still finding that my surface requires significant RO sanding with 120 grit to get out all of the surface blemishes. The blemishes generally look like chipout on the end grain, or perhaps it could be grain tearing and compressing? Either way, it's not up to snuff! It's do-able... but I'm getting tired of the extra work!
In areas of pure end-grain it happens everywhere. However, in areas where there are curves slowly transitioning from end grain to face grain it's often only on half the thickness. What I mean by this is in places where the milling that was done from the top has the blemishes, the milling from the back won't, and vice versa.
Note: I do the onion skin as the surface left from the initial passes is even worse. I attributed this to the bit being deep in a confined channel, often with debris despite upcut bits. Hence doing the onionskin at least gives the bit .015" breathing room on the final pass.

Problem 2 details:
As mentioned above I'm milling half my thickness (total 1.75") from the front, flipping things over, and milling the other half from the back. I have index pins (1/4") that allow me to accurately register the piece when flipping it. Again, bulk of the work is done with profile climb cuts and then the onionskin pass as conventional to get an 'as good as I seem to be able to get so far' surface. However, where these two passes meet in the center of the thickness they never seem to be perfectly lined up! I just measured and the current piece I haven't sanded yet, this is a .005" difference. But it's been bigger. Would estimate up to .010"?
My first inclination was that the bits weren't square to the table... but a quick check with a long bit and a good square makes me not think this anymore.
I then thought back to when I read somewhere that bits will deflect due to rotational forces... and that they'll deflect in vs. out depending on climb vs. conventional cutting? Could this be the cause of what I'm seeing? If so, is my only choice here to bump up to larger diameter (lower deflection) bits for this work?

Thoughts?
Chris

[coryatjohn]

Deflection is additive across your entire tool. Every part that has any flex, which is the entire machine, does so when placed under stress by the cutting operation. Slop in your bearings and adjustments can add up to a pretty good error. Going to a larger bit will likely not help much as it will only address the last link in the chain.

Perhaps you're thinking too much and not using your senses to judge what speeds and feeds you should be cutting at. If the machine sounds like you're milking a cat, then it is likely something is off.

Don't overlook a dull cutter too. A good quality solid carbide end mill should give you at least 20 hours of service, however, any abuse will cut that service life to a matter of minutes. Check your cutter carefully. If you see any chips taken out of the edge, or if it doesn't feel sharp, it probably needs sharpening or replacement.

An end mill clogged with gunk can also cut poorly. Be sure it is clean and free of debris and gunk from previous usage.

[dlcw]

Chris, I've found that when cutting there is a way to compensate for the inherent deflection in the Shopbot machines. I remove all except 1/32" material using a climb cut. Then I remove the final 1/32" material using a conventional cut.

The climb cut pushes the bit away from your cut line. The conventional cut pulls the bit toward the cut line. When I started making a living with my machine, about 9 years ago, I had a less then stellar first experience cutting cabinet parts in plywood. One of the great guys on here turned me on to the method explained above and since then, when cutting plywood, softwood or hardwood, I use the same method and the results have been excellent. The edges on my plywood are ready to go straight to the edgebander with nothing more than brushing off the dust. No sanding, nothing. Hardwood and softwood requires a little sanding, but not much.

Granted you have to make multiple passes but the time spent doing that are offset by not having as much sanding after the fact. The beauty is when I create the cut files, I include the climb and conventional cuts into the same file, saving pauses in the cutting process. I used to use a 3/8" compression bit to cut out everything, thinking that would fix deflection problems. All it did was cost more money. I do 99% of my parts cutting (plywood, hardwood and softwood) using a 1/4" compression bit.

But as the previous post says, make sure your bits are SHARP!! I gave up resharpening bits years ago. When making a living at this woodworking thing it's not worth the effort and the bits never achieve factory sharpness. I just build the cost of bits into the project. Now, saying that, when I decide to "retire" and do woodworking as a hobby, again, I might rethink the "always new bits" approach and look into resharpening. I'll cross that bridge when I come to it.

[verhoevc]

I did some more experimenting by milling slots and circles at .4" deep in two passes. I tried a .005 and .007 chipload (per onsrud recommendations) for both my single-flute bits (one new, one 'old-by-comparison') at 18k like they recommend instead of my usual 12k RPMs. They all sucked. Especially the circles! Got what horrible chipout! Lots of obvious vibration marks on surfaces, etc. This was with 62-727 and 63-727 bits.

I then threw in the 2-flute 57-910 and ran it at 180IPM=18000X2X.005 and here's what I saw:
- The machine SOUNDED much happier cutting
- The finish quality was monumentally better!
- HOWEVER: what I saw coming off the machine looked a lot more 'dust-like' than I saw in my other tests... which seems odd given the chipload calculation
- I'm going to have to up my hold-down game when running at these feeds... which perhaps is part of my surface-quality issue to begin with...

In conclusion... is are the 62-700 and 63-700 series bits just horrible choices for cutting wood?! I do see they don't appear anywhere on the wood chipload tables from onsrud... but they were some of the only single-flute bits I could find in the sizes I needed. I wanted single-flutes so I could run lower feeds while learning and experimenting with hold-down methods.

Chris

[verhoevc]

A little more info since I've been spending the morning experimenting. I've found that for the 57-910 I'm indeed getting nice surfaces in the recommended range; small success! So I've been doing more experiments with that bit instead of the 62-700/63-700 ones... but I'm still a bit confused...

I made a little maze for the bit to run curves, zig-zags, and straight lines across both face and end grain in a small 4x8" area. 0.3" depth over 2 passes in conventional cut in poplar.
Test 1: .005 @ 18kRPM= Nice surface but chips looked a little small/dusty, especially after in came back through for the second pass (didn't have dust collection on so I could hear/see better)
Then immediately ran:
Test 2: .0065 @ 13.8kRPM= Slightly less nice surface, but still not bad. Better looking chips IMO. BUT THE BIT WAS DEFINITELY HOT TO THE TOUCH AFTER! Putting a finger up against it for more than a second was not a pleasant experience.

How in the world am I getting a hot bit when perfectly within the recommended range (the top end even)?!

Chris

[verhoevc]

Anyone on problem 1?
Chris
PS: Thanks Don for the info on deflection eg: Problem 2!

[coryatjohn]

I had problems like you're describing when I first started working with my CNC machine. Of course, back then, I thought it was normal to have smoke pouring out when I was cutting with a handheld router.

The answer to your issues isn't math. It isn't science. It is feeling. You need to develop a more emotional relationship with your new machine. You need to feel when it is running right and when it is unhappy. That took me a couple of years and a lot of broken bits but one day, it all clicked and since then, I haven't broken a single bit. My cuts turn out as expected and I get repeatable results.

My advice is to keep experimenting. Forget about chip loads and calculations. Those things are created for industrial users with "big iron" machines. They really aren't applicable to these small scale CNC's.

Listen to your machine. Smell your machine. Feel your machine. Remember the rock opera "Tommy"? That's where the answer lies.

[EricSchimel]

To echo above, it takes practice. But, 24 IPM is WAAAY to slow to be cutting. You need to move faster. Go as deep as the bit is in diameter, and go at a minimum of 180. It's likely that faster speeds will give you even better cuts. Not sure what you have for a machine but 180 is good for both a Standard or an Alpha.

[bill.young]

It's funny but when faced with cutting problems, most people's first instinct is to speed up the rpms and slow down the move speed. That's almost always the opposite of what you actually want to do.

[verhoevc]

Thanks guys!
I'm usually pretty happy to experiment. My concern here is more financial than anything else. I'm currently using 1.4" bits (relatively cheap enough), but would like to upgrade to some 3/8" and 1/2" bits. If I'm going to blow through tools by pre-maturely dulling them due to incorrect feeds/feeds I'd prefer to get that out of the way on cheaper stuff hahahaha.
Chris

[coryatjohn]

By 1.4" I'm guessing you mean 1/4".

You are going to break end mills. That is a given. When you get to the point where you don't is a matter of experience. I suggest not using Onsrud bits for your testing. They are way expensive and give no meaningful advantage at the stage you are in with your experimenting. Buy some cheap end mills from Amazon or Ebay with no brand. You can pick them up for $10 or less each.

[EricSchimel]

If you're running the right feeds and speeds unless you run over a clamp it something you shouldn't be breaking bits.

If you're in the ballpark for the right feed and speed you won't break anything. Right now you're not even close to being in the ballpark :)

I'd follow some suggestions here on what people are running and start with those settings. Onsrud had decent phone support too. You can always call them and ask them about feeds and speeds.

To echo what Bill said... Spinning faster and moving slower is not the way to get better cuts and more life out of you're bits... Somewhat counterintuitively it's the opposite. Crank up that freed rate and drop your spindle speed!