Help needed! Cutting two-sided white 3/4'' melamine

[Nate Sirek]

Hi All,

I'm looking for some advice with cutting 3/4'' melamine.

We are a cabinet shop using a PRT Alpha with a spindle to cut box parts with a 1/4'' Onsurd bit up/down combo @ 3 inches per second at an RPM of 18,000 in a single pass.

We use a 6hp Spencer Regenerative blower on our vac table and parts don't move.....However when I put a tape on my parts they are getting 1/32''-1/16'' big and at the end of each side (by the corners) they dip in a bit to the correct size. Am I just setting my feed rate too fast? When I spoke to Onsrud they suggested 18,000 RPMs at 8.0 inches/second and I'm not anywhere near that speed @ 3'' per second.

Just looking through my manual I found some things about ramping as it pertains to cut quality issues but I'm a bit confused on what I should tweak my settings to. I get a nice clean chip free cut at 3.0 inches per second but it dips at the corners not all that different looking then snipe at the end of a board when it comes our the the planer.

[knight_toolworks]

are you doing a climb cut? usually parts are too small with a normal cut.

[beacon14]

Do a search on climb vs conventional cutting, or rough pass and finish passes, or look here (http://www.shopbotblog.com/index.php/2007/08/almost-there/) for an explanation.

[gene]

I would go up to 5 ips . i cut 3/4 plywood at 5 to 6 ips full depth compression cutter with clean edges at 13000 rpm on a spindle

[Nate Sirek]

Steve -- Not entirely sure if I cut it conventionally or with a climb cut. Without being at my shop I can't pull up my Partworks file to look at the logistics of my toolpathing.

Unfortunately I have a wedding to attend today that will keep me away from work but I plan on going in tomorrow to dig deeper into the issue. We bought our Bot a month ago used from a single owner (less then 40 hours on it!) and after using it a couple times having to clamp and screw down material we had just decided to wait to use it until our vacuum table was up and running. Well now it is and I can't wait to do most of my sheet stock machining on it.

Dave -- I read your thread about conventional/climb cutting and rough/finish passing. Is there something to Partworks that will let you call out over sized rough cuts and then a finish pass or do you have to create two separate toolpaths with different size vectors for cutting?

Gene -- I will bump up my feed rate to 5 or 6ipm and see if I notice a quality difference. I know Dave's thread explained how he cuts in two passes, are the rest of you utilizing this technique for cutting your sheet goods?

[knight_toolworks]

Most likely you are doing a climb cut. If you change to a conventional cut the parts will become smaller. but you can set a offset to compensate. that will be more consistent as a climb cut will bring out the worst slop in your machine.

[gene]

I use Ryan s program cabinet parts pro and it is set up to cut in a single pass. Yes it could be changed but it works good for me like it is

[paul_z]

Nate,

The "dips" are likely to be where the machine is decelerating to make the corner.

Using a 1/4" bit to cut 3/4" in one pass seems too much to me. I'd cut in two or three roughing passes and then a final full depth cleanup pass. The roughing passes can be cut at high speed because you don’t care about the quality; you’re just trying to get material out of the way so you can make the cleanup pass.

Use the allowance offset on the roughing passes. Perhaps 0.075". Then a cleanup pass with allowance offset to zero. I would also cut the cleanup pass at maybe two inches per second. As you get a better feel for your machine, you can probably increase the speed.

I’d also suggest that with the machine powered up but not moving and the spindle/router disabled, try to move collet on the spindle/router side to side in both the X and Y direction using about 20 pounds of force. It should feel dead solid. If not, you have a mechanical issue that needs to be resolved.

Paul Z

[curtiss]

Are not bits for making cabinets usually 3/8" in dia ???

Maybe something like this ?

http://www.vortextool.com/index.cfm?fuseaction=category.display&category_id=31

[beacon14]

I use 1/4" compression bits with good success. I cut at 5 ips, full depth (less the onion skin) at 14K or 15K RPM. The 3/8" cutter would have less deflection, but it also creates more sawdust, and the wider kerf causes more vacuum loss and lower material yield. Deflection with the 1/4" cutter is not an issue using the climb/conventional approach, since the sideways load on the final pass is uniform and minimal. 2IPS for the final pass will yield nice results at first, but the heat buildup will cause the bit to dull prematurely. Best to cut as fast as you can, with the lowest spindle speed, while still getting an acceptable edge.

For climb/conventional you have to use two separate toolpaths in PartWorks, but you can output them to a single file, and you can save them as a Toolpath Template for repetitive use.

Your best bet is to put a damaged or leftover sheet of material on the machine and do some test cuts to determine the best results you can get on your machine.

[Nate Sirek]

Well I had some time to run some test pieces yesterday without much success. I bumped up the feed rate to 4ips and lowered my spindle to 14000rpms. Tried a few climb and conventional cuts and haven't figured out too much. There isn't any play in my gantry. The cuts are good on both sides but still having some dipping and sizing issues. I'm not sure what to do other then keep making tests. Shopbot tech support just told me to check the gantry which I've checked multiple times and seems firm.

I'm thinking of lowering my speeds but I really don't want to jeopardize bit life length as well as speed of production. When I first bought this machine I didn't have a vacuum table so I was cutting all my pieces in 3 passes with dead accurate sizes and no dips. Then I couldn't take running screws and using clamps any longer so the vac table was essential. Now to just dial it in....

I'm getting a lift of melamine today for a job so I can run some more test pieces tonight when I have some free time (unfortunately I'm off to install all day today).

I Hope I can figure it out quickly and get this closet (first official cnc work project) turned around. I think this machine is an awesome investment, and when I bought it I kept telling myself "keep calm, read as much about it as you can, and don't expect to be making tons of money with it right away." Well its been 2 months and its killing me to not have it running more then it is! I wish I had another guy so I could focus on keeping our equipment running efficiently while not having to sacrifice production speeds. Why didn't god create us with 4 hands? :)

[garyc]

Nate...
This is most assuredly a deflection issue. The changes at the end are a result of going into ramp (slower) speeds, which reduce the deflection. IF you are still cutting using 3 passes the deflection is in the machine. If using a single pass it could be a combo of both. A dull bit would exacerbate the issue.

If the deflection turned out to be in the bit, cutting down to .030 from the bed in climb direction and following that with a full depth conventional pass will cure the problem. If not, then your machine needs adjustments.

If you post a pic of one of your corners that show the change AND the X and Y direction as the sheet is cut we can tell you what would be the first adjustment to make.

The problem is in your pinion to rack and/or V roller adjustments. The adjustments to bring these into specs are in the manual. Or call tech support and we can point you to the proper section.

In my prior cutting with an alpha, I would run a 1/4" compression bit near 6 ips @12,500 rpm full depth (onionskin) thru plywood. A 3/8 at 8-10. Your mileage may vary

[Nate Sirek]

So today I was using the same bit that I was experiencing cut quality problems with and it broke.

It broke making a 0.7075'' deep climb cut pass through 3/4'' mdf (old tables spoil board) to make some more tests. I'm really hoping it was having these issues due to the dull bit. It made a weird quick sort of thump noise and was sticking out of the board right next to the path it was cutting.

I wasn't able to make it back to the shop tonight after install to make more test cuts; however, I did have time to go grab a few new bits.

The only bit the local guys had was a Southeast Tool single flute 1/4'' compression bit so I grabbed it and ordered a few more Onsrud 1/4'' two flute compression bits (they'll be here Thursday).

If it doesn't seem to fix the problem I'll post some pictures on here if I can or upload them to Shutterfly for viewing.

[gene]

With the single flute i would NOT cut at 5 to 6 i would go back to 2.5 to 3 @ 13500 . By using a single flute you doubled your chipload over a two flute

[Nate Sirek]

Alright Guys,

This morning I changed to my new single flute compression bit and cut some test pieces as well as some shelves I had laid out in Partworks for a job we just finished.

I cut three sheets of 3/4'' white two sided melamine. Set the machine to cut the first pass at 0.7075 inches deep with a climb cut, and a final pass at 0.77'' deep with a conventional cut at 2.75ips at 13,750rpms. No offsets. Everything cut to size perfectly. I'm planning on checking my z axis for level/square just to double check.

Thanks to all of you for your advice, now just a couple more quick questions...

In regards to setting offsets....don't bother as long as part sizes are coming out correctly?

Second, what are your thoughts on using the same 1/4'' compression bit for drilling shelf pin holes with my spindle or doing dados? Some say you shouldn't other say they're doing it. My z move is set @ 1.00. I would like to do everything for milling my box parts with the one bit so to not have to do a tool change with every sheet (need and want the changer! 15k is hard to stomach though). Once I have a changer I could put in a different 5mm bit for drilling as I prefer 5mm shelf pin holes, but again, I'm inclined to sacrifice the 5mm for 1/4'' shelf pins if I can get by doing all milling steps with the same bit.

Lastly...Dave, where did you get the air clamp/suction cup parts for your sheet stock crane? I've got to make one of those!

[jerry_stanek]

You could peck drill

[gene]

I would not drill shelf holes with that bit . If i needed 1/4" shelf holes i would do a pocket toolpath with a 3/16 bit. If you drill 1/4" holes with a 1/4" bit it will create too much heat and puts too much upward pressure on your spindle. I tried 1/4" bit for drilling and caught my bot on fire. also too much upward pressure is bad for your spindle bearings.

[beacon14]

Ditto that. Compression bits are usually not made for straight plunging, they tend to burn up quickly, in which case you will still be changing bits more frequently. They have mostly downcut geometry, which prevents the chips (and heat) from clearing.

[Nate Sirek]

So what are you guys using to drill shelf pin holes? Everybody have air drills? Is there even a way to drill shelf pin holes with a spindle or is it just something to avoid?

What is peck drilling?

[bleeth]

I use a 5mm compression bit made to plunge from Centurian on my spindle. No problems. I also use peck drilling whis is drilling the hole in a couple of passes with a retraction to the surface of the part between downstrokes to evacuate the chips and keep the bit cooler.

[beacon14]

I use a second Z axis with a 3/16" downcut spiral to rout my 5mm holes - they come out perfect.