Searching for the perfect cut

[richards]

What would be the steps necessary always get the best cut from a Shopbot? These are the steps that I think would have to be taken to get as close to perfection as possible.

1. Verify that the Shopbot is in excellent working order.

2. Secure the material being cut so that it couldn't move.

3. Set the feed speed and router/spindle RPM to get the desired chipload

4. Use as large a rough cutter as possible to cut the part oversize. Oversize meaning 0.20-inches or so greater than the jitter or chatter produced by using a rough cutter. For example, if the jitter were 0.04-inches, the part could be safely rough cut 1/16-inch oversize.

5. Use a spiral cutter for the final clean-up pass. Use the feed speed router/spindle RPM suited to the material being cut and to the desired surface - assuming that a cut at 1-ips would give a smoother edge than a cut at 10-ips.

The reason that I'm asking, is that some of my construction clients are perfectly happy with a cut that is within 1/4-inch. I can easily hold 1/8-inch at full speed with a single-flute straight cutter. Another client wants the perfect edge finish. For him, I'll need to have a reasonable way of listing the steps necessary, and the time required for each step, to give him the best result possible from the Shopbot.

Any ideas?

[gerald_d]

Sharpness of the cutter should be in the list as well.

[tuck]

"Sharpness of the cutter should be in the list as well."

That may well be the single most important thing. It's like slicing tomatoes with a dull kitchen knife if your bit isn't good and sharp.

[greg_russell]

Mike,

When you say "rough cutter" what kind of cutter are you referring to? Do you mean the single flute you referenced?

[richards]

For my use, a rough cutter would be a single-flute 1/2-inch or 3/8-inch straight cutter, although the Onsrud 60-000 series hogging cutters look very interesting. For definition purposes, a rough, hogging cutter is a cutter that, in one pass, would get me close enough to final size that a finish cutter could take me right to the line, in one pass.

I agree that a sharp cutter will cut while a dull cutter will tear or burn its way through the cut. At one time, Eric Lamoray suggested watching the Amp readout on the spindle's VFD to determine when a cutter is getting dull. That works well for me.

[jhicks]

I don't think I have the answer but can bring this to the table. In discussions with Onsrud about this subject, I was cutting 3/4" poplar and needed a smooth edge. I tried the offset and then an overall .020" final pass to clear the edges but still didnt see what I wanted using .25" 2 and 1 flute spiral end mills and O flutes. The Onsrud folks told me that .020" wasn't enough of an offset. That that .020" or .025" offset simply wasn't enough for the final pass to load the bit and more likely just caused more bit deflection along the entire depth. They recommended a more aggressive offset and final pass depth to load the bit and give it more material to cut/hold the bit on the bottom and perpendicular to the stock. In our case we were leaving an .025" onion skin so the bit never hit the table/spoil board.
In the end we used an .050" to .070" offset, and a .250 final depth pass, plus slowed the move speed down and improved the edge considerably but I can't say it was perfect, just better. O-Flute seemed to give us the best over the 2 flute end mill but we really don't know why. Maybe better chip clearing is all I can figure.
It seems the combination of variables makes achieving a perfect edge so sensitive to every nuance that a final sanding step is always required for us. Hope you find the answer.

[richards]

Jerry, leaving more waste during the rough cut pass makes a lot of sense. In my pre-shopbot days when I used templates on a shaper and on the router table, I usually got a better edge finish when the bandsaw cut was at least 1/8-inch oversized.

My goal is to get the smoothest edge possible using two passes. Pass no. 1 will run at the highest speed possible, depending on the material and cutter. Edge quality on pass no. 1 is of no concern, as long as it can be fixed on pass no. 2. Pass no. 2 will cut the part to proper size and fix the roughness left from pass no. 1. Pass no. 2 will also be run as fast as practical; however, the actual feed speed will be chosen to most closely match the customer's quality expectations. For example, if a feed speed of 2-ips gave a near perfect edge that requires almost no sanding, while a feed speed of 8-ips gave a good edge that requires slightly more sanding, the customer could decide whether he wanted to pay for the extra CNC time required to cut slower or pay someone to sand the parts.

I think that the basis for this thread is to verify that I'm following a repeatable process that will produce the expected results in the least amount of time. If the process is repeatable then several grades of edge smoothness could be offered - at prices that reflected the CNC time required to produce those edges. Instead of telling the customer that the parts will be pretty accurate and pretty smooth, I'll be able to show samples knowing that the customer's parts will have the same edge smoothness as the sample parts.

[jhicks]

Mike, given similar curcumstances, we did just what you described. Ran probably 4 to 6 variations to see the impact and variation, then provided them 3 options for final approval. Time really didn't change that much but the better edges were the slowest final pass cuts.
Accuracy wasn't the issue but IF the final parts need sanding to clean the edges, I think an extra .005 offset on the outside cut is about right to compensate for final sanding finish.
Seems trial runs and documentation are key but with a piece of wood, and an entire cut out, chances are you will see variation between end grains and along the grain cuts. Even the opposite sides with end grain cuts will reflect essentially a climb on one side and a conventional on the other so we never arrived at perfection assuming that's defined as no sanding.

[drodda]

I will start by saying that I don't have a spindle yet.

I will wait while you evangelical spindle greater than though make your coments at your computer. Go ahead nobody can hear you anyhow.


Ok back to the post. I have found that even cutting two identicle pieces out of the same piece of wood do not end up with the same edge look. I have been fighting this for some time. I have blamed this on my router but would like to know do the spindle guys have this same problem or can you get exactly the same results given the same wood and speeds every time?

I have many more questions but out of respect to Mike's thread I will ask the rest in a new thread.

[rhfurniture]

I think that the issues are COMPLETELY different for solid wood with a grain direction - often variable, and partical board, or even plywood where the grain induced forces are even.

[richards]

It would be nice to cut wood. All that I cut is glue with a little sawdust mixed in.

[jhicks]

Dave,
I agree with RH about the natural wood vs more consistent materials.
I find that when all settings are square, hold downs are solid/flat, and speeds are dialed in, parts do cut equally. This photo is of a stack of 8 1/2" MDO sign blanks made for a local vinyl shop. His jig saw just can't compare in any way plus his vinyl fits exactly over the panel since we both cut from the same vector files.NO WAY he could accomplish this with anything except a scroll saw and even then there would be variations between pieces.
This is the type of "Value" pricing vs time and material I was referring to in the "CNC proliferation" thread

These were cut with a .125" end mill, around 13,000 rpm at a move speed around 2.0" / sec with a final pass thickness of .080 and nothing holding in the panel after the cut except the packed chips.
When laying one on top of the other to compare before delivery, they matched perfectly and edges were consistent.
It doesn't seem to me that Router or spindle should really matter except perhaps that the spindle can be dialed in at any RPM incrementally vs a typical Porter cable at only predetermined speeds. Of course overloading the router, slack in the bearings, or anything else that might have excess play would be a negative even with a spindle.
That said, each piece of natural wood has so much grain,moisture,and density variation in all directions that I guess one must expect edge variation and try to get the best overall cut possible.
I do wonder sometimes if a "flush cutter" would do better at this than an end mill or 0-Flute but haven't tried it yet. Probably need to run some comparisons on that.
5225

[don]

I have the luxury of grinding/manufacturing my own tools. After expermenting with tool geometry. Here are a few parameters that has helped solve some of my chatter\jitter.

Here is process when making my FINISH tooling.
When fluting the blank,I've made sure that I've increased the rake of the flute to about 12 to 14 degrees instead of the average 9 - 10 degrees. I also increase the spiral\helix. Usually 30 degree to a 40 degree. Along with having the largest core diameter as possible. core diameter = tool diameter - (flute depth * 2) I try to keep core diameter approx 60% of total diameter. ( larger core diameter makes the tool stiffer and to flex away from the part while machining.

After fluting, I remove it from the machine then polished the flutes to a mirror like finish. (polishing\buffing wheel on a bench grinder w/polishing compound) It makes the flutes really slick and don't have the problem of any type of material sticking to the tool.

After fluting and polishing, I've chucked the tool back into the machine and then ground the primary and secondary reliefs on the diameter and ends. Giving the diamter primary more relief. 11-12 degrees (average .500 tool is 10 degrees) This increase in rake, primary diamter and helix/spiral geometry works more like a sharp scissor cutting instead of ripping, giving me a cleaner, smoother cut.

I know very few have access to grinding your own tools. But there are local tool grinders every where. And they can manufacture\regrind the tools to your specs. Just like the botters can make projects to their customers specs.

I try to leave .030-.040 for my finish pass.

Don't know if any of this helps, but hope it gives some insight.

Don

[richards]

Don, am I correct in assumming that you're making your tools out of high-speed steel - not carbide? I understand that high-speed steel gives a better finish than carbide, all other things being equal. What do you think?

[gerald_d]

Hi Don - very, very interesting! That is something that I would like to do as well. What type/size tool grinder and stone do you use. (This might de-rail Mike's thread a little - sorry for that Mike)

[don]

Mike:
We make both HSS and Carbide. I like to use Carbide because the cutting edge doesn't break down as fast as HSS does under heat. The finish of the tool is also controlled by the operator via spindle speed( wheel speed)and grit and compound of the wheel.

Gerald:
I've been known to using a snag grinder at 3am in the morning to get a job out the door if I don't have any sharp tooling. But at my day job (really 2nd shift)We have 2 brands of cnc grinders. ANCA (http://www.anca.com/pages/default.cfm?page_id=22557) and Walters (http://www.grinding.com/machines/pages/content/machines_cutter_walter.html) Not trying to advertise for these companies, these are what we use. The links may load slow.

We use Diamond wheels for carbide and CBN Borazon wheels for HSS.

Yes I hope this doesn't derail Mikes thread.
Its just that I've gotten so much information from all of you proffessionals, I thought I'd toss in what little I do know.

Don

[richards]

Don, Your information is welcome. If grinding the cutter differently from standard commercially available cutters gives a smoother edge, then we have another way to improve our product.

After looking at your links, I can easily see how you'd be able to make a customer cutter. There is a shop here in Salt Lake (AA Carbide) that custom grinds CNC cutters. In the past, they've been my supplier for Whiteside and Onsrud cutters. Until today, I'd never thought about looking into having them make a custom cutter.

[dirk]

Don

[don]

Dirk,
Yes it will work for both roughing and finish pases. Your correct I stop and change tooling for the finish cut only if the project require a smooth finish or can be sanded with little effort.

Mike and Dirk,
I have had a few jobs where it was worth making a special tool to keep from changing tools. It all depends on the profile of the pieces.

Here is a rough drawing of a tool I had made to run this job of 200 pieces. The part 1" celtec and 24 x 18 ellipse with a profile. I made 5 tools in case I had to run over the weekend. The tool also had 3 flutes with a 30 degree spiral.
Sometimes its cheaper to have a special tool made to save time in the long run.


5226

This may not be fit for this thread. But I'm also making a tool to attempt to machine inside and outside threads on 8 inch diameter piece. A large contain ( possible a cookie jar )I haven't decided yet. But will be using the CC with the spiral parameter to cut the threads on the lid and jar.
Am wondering if anyone else has attempted this. If so I'm all ears.

Don