Cutting Melamine

[todd@miterwright.com]

We are using an Onsrud 3/8" compression bit for cutting 3/4" melamine.When we cut in two passes the down cut part dulls after about 5-6 sheets, but if we cut in one pass, the Y axis loses position. Does anyone have any suggestions on how to remedy the problem? I was told by Shopbot to cut in two passes but I was told by my sharpener that these bit are made to cut all the time and to cut in one pass.

[elcruisr]

We cut a lot of 3/4 melamine in one pass with the same type tooling. Are you using a single or double flute? What is the feed speed and rpm's? I should be able to help you if you can give that info. It should last through an 8 hour shift not a few sheets.

Eric Lamoray
Balsys Wood Arts, Inc.

[robinsoncr@naxs.net]

Todd,

We tried several brands and styles of bits before finding an acceptable combo. We do 95% 19mm two sided melamine. Our setup is as follows:

5hp Columbo Spindle @ 10,000rpm
MS = 1.67,1.0
Onsrud 3/8 Compression Mortising Sprial, 1 flute
Single Pass Cutting

This setup was obtained from a tool engineer at Onsrud and it has given us the best performance.

Chris Robinson

[dmdraper]

Onsrud has excellent tech support and also feeds and speeds charts on their website, you may want to consult them. Feed and speed are critical with respect to cutter life. With downcut spirals, chip removal is also critical because a lot of heat is carried away with the chips. If your tool path is pack with chips, your bits will wear out long before they should.

[Todd (Unregistered Guest)]

I'm at 13000 rpm, MS 1.75, 1.0 Onsrud 3/8 compression double flute, not sure of the model number. Thanks for the help.

[Todd Salony (Unregistered Guest)]

What programs are you guys using? I'm using Part Wizard. In your programs does the bit go back and forth while plunging? I'm not sure if you can do this in PW. Thanks again, Todd

[elcruisr]

I'm running Artcam Insignia for toolpathing and CAD. Ramped entries and leads are very important for spindle bearing life, tooling life and part quality if you're doing production work. You could write a small subroutine to do this at the start of each entry if nothing else.

We ended up running at 2.3"/sec on x and y and 1.3 on z. We do have double y motors and this helps the speed a bit. Typical rpms would be at 10,000 with a single flute. The double flute you're using is more flutes than you can use at the feed speeds we can reach. That means more heat is being generated and heat dulls bits very fast. I've learned this one the hard way myself and from the tech rep from Onsrud who came to the shop.

Onsrud makes single flute compressions in standard and short up cut configuration which we like for smaller parts as it exerts more down force to keep parts on the table better.

Eric

[pcathome@telesal.net]

We are cutting 5/8 double sided melamine with 1/2" and 5/16" with 1/2" shank, but we always get inconsistent sizes.
If we cut many pieces of the same size in the same panel, they are never equal to each other by 1/2 mm or even 1 mm

We have tried cutting all the vertical lines first and then horizontal to make sure that horizontal sizing is not influenced by movement of a poor vacuum holdown, but still size is off by 1/2 or 1 mm ???

[gerald_d]

Alberto, if you are cutting panels side by side, and your "verticals" are cut up and down as in the sketch.....


4711
...... then panels A & C will be "wide" and panels B & D will be narrow due to deflection of the bit and gantry. If you cut them all "up" with the same load on the bit, then they should be identical.

[hwd_woodworking]

Alberto,
Initially when we set up our machine we had the same problem. Two things to check first...

*How sqaure is your machine, We square our machine by first putting in a v-bit then run a drill routine on the four outside corners. We then through the software un link the two x motors and make the corrections by moving only on x motor. Re link them then run another four corner program. (PS don't shut your machine off, leave it on all the time).

Second check all the bearings on your gantry in various y positions. You may find that as the spindel moves in the y direction some off your bearings become loose.

We initially had the same problems and got far better results after keeping a close eye on those two things.

Also what Gerald d said is true. If we use that method we make sure all our vectors are cutting in the same direction in both the x and the y.

If we were to run a profile test such as cutting 5 rectangles. roughly 12" x 18" one in each outside corner and one directly in the center. Our rectangles come out very close, when stacked on top of each other. They are not perfect, but you can barely feel the difference. I believe if we get an additional y motor it will further push our tolerances.

There are other things that could be contributing to the unequal panels such as splitting motor pulses.
We notice that when we make a divided mail cabinet with 3 1/2" cubbies made out of tempered masonite that slide into 1/4" grooves. The slots must be cut after on a jig that is positioned on the shopbot. What we found was if we cut the grooves first then profiled. We saw a pattern develop like the first two grooves were fine then the third was a little wide ect... Because we need to match the grooves on pieces that are also cut from the other end of the sheet (due to many shelves) the grooves won't be perfectly aligned.

We have come up with temp solutions like cheating a vector in the x direction to compensate for this but that only helps us if we are making duplicates.

Nate

[mnrite]

I am going to cut some melamine right on the vacumn grid (no spoilboard) and use a skin to hold the parts in place. How do you separate the parts without damaging the bottom melamine. Break them apart? Flip the sheet and route them apart? Slide the sheet off the grid and route them from the top? I am going to try all the above but was wondering what others do?

Thanks
Mike

[Brady Watson]

Mike,
If you put a layer of Trupan or Pro-quality MDF or LDF on top of the grid life will be a lot easier. Then you can either cut all the way thru or bridge the start point of your profile if necessary.

-Brady

[richards]

I cut almost through, leaving about 0.050 inch and then use a plastic laminate scoring tool to score the cut. At that point, the material is either cut free, or easily snaps apart along the scored line.

When I've tried to snap melamine apart without first scoring, it tends to snap right at the edge of a cut which usually means that the edge is chipped and ruined.

[mnrite]

Brady - I don't think I have enought vacumn to suck through a spoilboard. A Rigid shop vac and I want to cut up full sheets.

Mike - do you score it while it is on the grid, or slide it to another table to protect the grid while you score.

Thanks
Mike

[seana]

Mike E,
I think you would be surprised with how well a shop vac works.
I use a Ridge shop vac and have it running 4 zones with 1/4 mdf spoilboard and i can cut full sheets no problem.
In fact with small parts i hot melt glue them on to a piece of 1/4" mdf to cover the vac zone and still get pull through both pieces, 1/2 of mdf.
Really give it try. I can lift the piece up with out a problem but i can't push it across the table.
I have found when cutting melamine i do an offset of all most .0625 and cut in 2 passes and leaving a skin of .0625 and then do a final pass full depth to the size that i want and the shop vac works great.

Sean

[richards]

Before I used a spoil board on top of the grid, I scored it while it was still on the table. The scoring tool nicked up the vacuum platen.

I've had no trouble using a spoil board on top of the vacuum platen with my Fein, but I rarely have enough vacuum to make one-pass cuts in melamine. The panels don't slide very much, usually between 1/16 and 1/8 inch, but that's too much for the 32mm system that I use where the edges have to line up perfectly. Until I can greatly increase the vacuum, I've gone back to making a partial cut leaving about 0.050 inch so that vacuum is held on the entire sheet.

If you decide to NOT use a spoil board, you might have to leave a skin about between 1/16 inch and 1/8 inch thick to keep the vacuum from breaking through the melamine.

Sean's two pass method should work perfectly.

[wemme]

Alberto I had a similar problem which was due to a loose bearing in the Y axis and was also cut direction dependent I.E. would cut mostly fine then somedays not.

[wayne_walker]

I am needing to drill a lot of 1/4" holes thru 3/8" ABS plastic. I am using a PC router on a PRT so speed control is limited.

I have tried an single flute, upcut spiral bit at 10,000 RPM with a plunge rate of .5 to 1. and the material tends to hang up on the top of the bit and marr the top surface. I best results so far have been at 16,000 or 18,000 and .4 plunge rate. Even then, I am not getting the best results. After a few holes it starts to stick to the bit again. I have tried higher RPM thinking it would throw the mertial off the bit but that does not seem to work.

Is it best to plunge faster and keep the PRM's down?? How fast can I plunge without damaging the bearings?

I'm going to set up an air drill on it when I get a chance but, I have to do at least part of this job with the router.



Any help is appreciated.

Thanks,

Wayne

[gary_n]

I would recommend using a down cut bit, either single or double flute. Your speeds should be OK.

[Brady Watson]

Wayne,
The drill is the right tool for the job obviously...and routers and most spindles are not rated for drilling (they sell spindles that are rated for drilling...the standard Colombo is not)..but if I had to drill plastic and the job was worth it, I would decreas RPM to 10k, and increase the Z-plunge to as fast as I could do it. The reason you are getting the top marring is because the plastic is heating up, quickly cooling and scratching the surface. If you have ArtCAM, peck drilling would help. If not, use an aggresive Z speed.

-Brady

[wayne_walker]

Gary and Brady,

Does the down spiral force the material down into the hole? Does it affect the bottom of the material? (melt back)

How aggresive can I be - 1.5 to 2.??

Thanks for the input.

Wayne

[Brady Watson]

Wayne,
I do not recommend a downcut spiral for any plasic over .0625" thick. It will weld the cips to the bottom side of the piece.

Get a piece of scrap and try drilling 10 holes in sucession at various speeds/feeds. I would try setting the Z speed at 1.5 and go from there. Also, to save time, set your safe Z height to .25

The other thing that you can try is using an 1/8" straight cutter and do an inside profile cut, stepping down 1/8" in each pass. See how clean the holes are. If they are not clean, just profile cut them to .23" and then drill stright down with a 1/4" bit. This will only take off .01" off of the sides and will probably not melt. I know it sounds like a lot of work...but it may be the only way to get clean holes given your equipment.

-Brady

[seana]

Wayne,
The guy that i purchased my bot from, used it to cut HDPE with drilling tons of holes.
He made a bracket to hold a piece of HDPE so when we pulled up the router from the plunge it pulled up through the scrap HDPE and cleaned the bit.
I think he mentioned he had to do this because the bit would be full of "chips" and reweld.
Sorry no pic's of his set up, and it was removed before i recieved the bot.
Hope you can make some sense of my rambling.


Sean

[gerald_d]

Sean, that makes a LOT of sense. Sort of a "pressure foot" like a sewing machine, where the foot also serves as a mask.....

[wayne_walker]

Brady, Sean, and Gerald

Thanks for the input. I will try the aggressive plunge at a lower RPM see how that works. I assume that if I plunge too fast, I will loose steps on the Z motor. This would be the best route for me, if I can get it to work.

I will also experiment with the 1/8" bit and see how that works.

I have thought about using a brass brush that could be used to knock the build up off of the bit at the top of the flutes.

Thanks,

Wayne

[gerald_d]

A good blast of compressed air might keep also the bit clean.