Help me out here. What is your:

• IPM (inches per minute)
• RPM
• Router Bit diameter
• Number of flutes
• Upcut, downcut or straight

Thanks

Andy,

For 1/2 material we use:

420 IPM for the 1st pass    450 to remove last .04

18000 RPM

1/4" bit

Single flute

Upcut  the down cut bit was forcing the shavings between the material and the spoil board.

John

Andy,

For cutting 1/2" solid surface we use:

250 IPM (one pass)

18000 RPM

1/4" Dia.

Upcut "O" flute

John,

Wow - 420 IPM is cruising. I imagine you are taking two passes to keep parts from moving. Does the operator still have to stop the machine to remove build-ups before routing the other parts? Do you still take two passes on large parts? On the second pass, are you taking any material off of the perimeter of the part or just dropping down .040"?

Rich,

Yeah, 1/4" dia. tool does the trick. A 1/2" dia. tool is overkill and will cause more pressure that will cause small parts to move easier. We use a 1/2" dia. tool mostly for plowing and for cutting faucet holes so the slug left from the faucet hole is smaller.

  Have a nice evening,

  Seth

Seth,

We cut all the pieces with two passes then remove the waste at the end.  First pass removes 95% of the depth then we kick up the speed on the second pass.  Using this method "onion skin" we have been able to cut some relatively small parts with no movement.  Took us a while to get a process down but finally got it.  We were cutting at 450 IPM but after a few sheet and the bit started getting dull it would break a little sooner than we wanted.  By going to 420 we get quite a bit of cutting from it.  We tried cutting slower with one pass but the chip load was higher and we got more movement even though we have a 50HP pump.  When we cut 3CM now thats a whole nother ball game.

John,

You cut all the parts nested on the sheet with the first pass at 420 ipm and 95% depth and then recut all the parts at full depth but increase the speed to 450 ipm

Doesn't that mean if I can cut the all the same material at 275 ipm, this process would be faster.

Just curious.

What is the average two sheet job time?  Mine is about 6-8 minutes.

We use a 1/4" upcut spiral @ 250ipm.  Could probably run it faster, but the machine only runs for about 4 hours most days, so it really isn't a constraint on production.  If we had more work, speed and optimization might become more of an issue.

Andy,

That seems really fast for two sheet cutting.  If I nest everything, sometimes it takes 10 minutes to cut one sheet....

I will have to time one out today.

We tried cutting in one pass but we were getting movement, too much cutting pressure.  so using 2 passes works well with no movement.  We can one pass large pieces, but for the CAD it is easier just to set one program up, copy it and use a different final depth.  Mind you this method is not set in stone, we try some different stuff on occasion.  Always open to suggestions.

3CM

250 IPM     3/4" rough cut up spiral 18000RPM        First Pass

350 IPM     3/4" finish up spiral     18000RPM    Second Pass

Matt,

Are you cutting every single piece for the countertops.  All the edges are included?

Yes Andy.

When I program a job, all build up edge pieces (1" wide double stack), loose splashes (with seams marked if necessary), trivets, cutting boards, cooktop corner blocks, warranty color match piece, anything else needed for job is in the program.  Scribe strips for cove, also.

It is easier to do it that way, so that everything is accounted for.  Too many times somebody forgets to rip something on the saw before it goes to the CNC or after, or when the job is finished, you are digging through the dumpster finding a piece for warranty purposes or splash that they forgot.

More work for me, less work for the guys, like always......

More work for me, less work for the guys, like always......

[/QUOTE]

Amen to that.  I feel like you just explained my job.

Matt,

We do the same thing.  The part I like the best is that it takes a lot of the thinking out of the shop and keeps it in the office.  My CAD guy has a master template with preset corner blocks, build up, accessories, etc that he can just drag into the drawing when all the main pieces are laid on the sheets.  It works well for us.  Like Andy said as far as the work is concerned but it makes the shop much faster.

John

John,

Thanks for the response. Not having to worry about parts moving, that would be nice. Our operator has to stop the machine after each build-up is routed, remove it, then proceed with the rest of the program. The two passes is something to consider.

  Have a nice evening,

  Seth

We had to do that in the begining too.  What we do now is called onion skinning.  On your first pass cut all but the last .04.  Starting points dont matter here.  The second pass cut all the way thru now is where starting points come into play.  We can cut perfect 1" strips all day and if your start point is right it will move but away from the bit after it is cut and wont get any damage.  Call me if you have any questions

(239) 334-1151

John

I single cut everything at about 275 ipm.  I cut clockwise starting with the outside pieces first.  Then I cut the small pieces away from the larger and work my way to the center of the material. I rarely have a piece move and I think I save a ton of time only cutting the piece one time.

Are there any advantages that I am not seeing, cutting the pieces twice?

275 ipm

18000 rpm

3/8" triple flute helix upcut bit

clockwise around inside and outside of parts.

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

 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

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.

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.

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