[John Cristina]

Andy,

You are cutting in a clockwise direction? We run opposite should we be running clockwise? What happens when you use a 1/4″ bit so there is less cutting pressure and waste? Call me when you have a minute, I have some more questions for you.

John

239-334-1151

[Seth Emery]

I was taught in school that climb-cutting, which is what Andy is doing by routing clockwise around the perimeter, should not be done when removing a significant amount of material. The only way that this would not be climb-cutting is if you have a left-hand tool and your spindle is turning counter-clockwise. Climb-cutting can cause the tool to “jump” into the cut. Since Andy is using a 3/8″ dia. tool and I’m guessing the flute length is fairly short, the tool is rigid and climb-cutting must not be affecting performance or I’m sure Andy would have changed things. Climb-cutting leaves a slightly nicer finish than conventional-cutting (cutting counter-clockwise around the perimeter), but I was taught to rough off material using conventional-cutting and then take a finishing pass of .001″ or less using climb-milling. That was for milling steel, so I don’t think the climb-cut pass is necessary for solid surface since we get a nice finish by conventional-cutting.

Using a 3/8″ dia. tool could really throw a loop in things for me. Nesting a 25-1/4″ deep countertop (due to overlay drawers) with 1-1/4″ wide stacked build-ups and a 1″ wide cove strip is normally fairly tight using a 1/4″ dia. tool. With the 3/8″ dia. tool, that would add another 3/8″ to the used material and adding any material for reintroducing would put me over the 30″. Also, I like to have at least 1/16″ trim along the outer edges. Andy, how do you deal with this? Order more material? Not make the build-ups 1-1/4″ wide even though the overhang is 1-1/4″?

Have a nice day,

Seth 717-917-3259

[Andy Graves]

Seth,

I have absolutely no problem cutting a clockwise direction. I you think about it, it you cut a straight line down the center of material, not mater what you do you are climb-cutting on one side. I am just putting the nicer finish on the side I want to keep. Maybe I am thinking wrong on this but that is the way it seems to me.

If I did the 1 1/4″ edge I would probably switch to a 1/4″ bit, but I usually only go up to a 1″ wide buildup. We allow our counters to hang down onto the cabinets to cover the old tile line. I can’t have the buildup sit on top of the cabinet.

John,

I don’t think climb-cutting is standard, I just get a better finish and have had no issues whatsoever. So I am sticking with it.

[Andy Graves]

John,

1/4″ bits break on me. I can’t stand that. Half way through a job and the thing snaps. I would rather have an extra 1/8. I don’t really have an issue with my parts moving. I have spent a lot of time trying to cut small pieces to large and I always cut the pieces to fall away from tha larger piece.

[George Owren]

Thanks for all the info. My CNC should arrive next week and I’ve been looking for this information. I did a lot of metal fabricating in my other life and am going to enjoy getting the CNC up and running.

George

[Shane Barker]

We also climb cut everything, CW spindle rotation, CW cut direction. I only onion skin the small parts and mostly just the build up pieces. I might give the ¼” cutter a try but I have good luck with the 3/8”. We have little problems with parts moving.

350 ipm (operator adjusted up and down as needed)

18000 rpm

3/8 two flute up spiral

25 hp Kaeser Rotary Screw Vacuum (550 cfm)

Shane

[John Cristina]

Shane,

We get less movement when cutting with a 1/4″ bit. There is less cutting pressure. After ignoring what the manufacturer suggests about spoil boards, we have been able to tweak our set up a little more. We cut all pieces at 400 IPM with no movement 18000 RPM. We tried to cut faster but the 1/4″ bit snapps at 420 IPM. We can not cut parts with a 3/8″ bit due to material useage. Have you ever fly cut your spoil board at 3000 IPM? Wish I could cut my parts that fast.

John

[Shane Barker]

John,

I don’t remember off hand how fast we do the fly cutter but I know it is scary fast. I was cutting PaperStone today with a 1/4 “ cutter at 350 ipm and after about 6 min. it snapped. But I think Paperstone is a lot harder to cut. I will give the ¼” cutter a try on our SS. Thanks

Shane

[Andy Graves]

I used to use 1/4″ bits and they would always break.

[Shane Barker]

I am not sure what the secret is Andy but it sounds like a lot of guys are using ¼” cutters. But it sucks to snap a bit when you are trying to get a job cutout.

Shane

[Andy Graves]

Yea and they are cutting a pretty fast speeds. I tried to figure it out, but with no luck.

[Shane Barker]

Maybe it’s all about the cutter. If someone can post a part number and brand of the cutter they are using we should have the same luck as they are having, or better yet someone should send me and Andy a cutter to try so we can see for our self.[EMO]bigsmile.gif[/EMO]

Shane

[Seth Emery]

Here’s manufacturer and part number for the 1/4″ dia. tool that we use for routing 1/2″ solid surface: Onsrud 63-725. We run at 250 IPM and 18000 RPM’s. I rarely hear of one breaking, but they aren’t worth resharpening when they get dull. If one breaks in the middle of a program there is a way to pick back up where you left off – at least on a Fanuc control. There are just a few things you have to be careful about when jumping lines. Shane, did they show you how to do that in your classes at KOMO? I don’t think they showed those who went from our company.

Have a nice evening,

Seth

[Shane Barker]

Seth,

Thanks for the part #; I was using a 63-776 which is rated for solid surface and soft plastics. I had it in stock so I tried it on the PaperStone and it didn’t last too long, but I never tried it on solid surface. The 63-725 is a little shorter and is for hard plastics and solid surface so it might do better on the PaperStone. I also think I had the feed too high at 350 ipm. I don’t remember being taught how to pick up on a program like you mentioned but our programs or usually so short that I will just reset to the beginning and re-cut the program. How do you start mid-stream?

Shane

[Seth Emery]

Shane,

Yeah, cutting 1/4″ thick material with 1-1/4″ flute length seems like it must be letting the tool flex too much, especially at 350 IPM. I would consider using the 63-724, since it only has 3/8″ flute length and you have a large number of parts to cut. Are you climb-cutting or conventional-cutting? I’d go with conventional, at least for the 1/4″ dia. tool. Starting mid-stream in a program is helpful when you have long programs and don’t want to run the whole thing over and when you get into profiling tops on your CNC. Do you do any profiling on your KOMO? Here’s how to jump lines – I’m just going to type in the pertinent info to save time:

Your tool from position #8 breaks at N30. Touch off a new tool. Reset the program and run in single block mode down to N9. Push the Edit button. Type in T2008 and press the down arrow. Cursor up to N16. Push the Mem button. Run in single block mode down to N21.Push the Edit button. Type in N30 and press the down arrow. Cursor up to N26. Push the Mem button. Run in single block mode down a few lines past N30 to be safe and your ready to go full speed. The important things are that you start and stop at the same Z position (.6 in this case), and that you make sure you pick up the proper tool. I’d turn the feed and rapid traverse rates down to a minimum just to be safe. The first few times you do this can be a little nerve-racking, but it gets to be worth it. Feel free to give me a call if you ever have a problem. I’d like to talk to you about a few things with Router-CIM and AutoCAD also. 717-917-3259

N1
N2
N3
N4
N5
N6T2006
N7
N8
N9Z.6
N10
N11
N12
N13
N14
N15
N16Z.6
N17
N18T2008
N19
N20
N21Z.6
N22
N23
N24
N25
N26Z.6
N27
N28
N29
N30X10.5Y10.5

Have a nice evening,
Seth

[Author]

Posts