MechMate CNC Router Forum

Go Back   MechMate CNC Router Forum > After Building the Beast - Operating , Troubleshooting and Maintenance > Cutting various materials - bit selection, feeds, speeds
Register Options Profile Last 1 | 3 | 7 Days Search Today's Posts Mark Forums Read

Reply
 
Thread Tools
  #1  
Old Wed 07 October 2015, 20:45
digger
Just call me: Milosh #113
 
Toronto
Canada
Melaine again

Hello fellow MMers,

It's been a while since my last post. I did some cutting for friends and family, and ended up in a community papers for a sign I made for a good friend of mine. I saved a black melamine table top and made a sign out of it for him. First time to cut a melamine for a sign and it worked just as it should be - no chipping. After that, cut another one, also, without chipping. Next one, is giving me hard time. Got the panel from HD and start to cut it and there is a problem - chipping. Melamine is made by a Canadian company - checked in a store. I assumed, the quality will be good, but it looks like, I was wrong. Have chips all over the edges. So, cuts were made with a 1/8" 2 flutes downcut bit, depth of cut is 0.04" speed 280 IPM and 10000 rpm (0.014 chipload), and 25% of stepover. Tried different cutting strategies, but no change. Different speeds, but no change. What am I doing wrong?
Reply With Quote
  #2  
Old Thu 08 October 2015, 16:17
digger
Just call me: Milosh #113
 
Toronto
Canada
Well, I did some research and found that there are different grades of melamine. Somebody is claiming that grade is based on core (glue, density...), but somebody is claiming that there is a difference in thickness of protective surface. I believe, truth is somewhere in between. Melamine from orange box stores is lower grade, and hence the lower price. That's what people are saying. So, to solve this issue, I guess have to find some supplier to get it from him.
Reply With Quote
  #3  
Old Thu 08 October 2015, 18:28
servant74
Just call me: Jack
 
Nashville (Tennessee)
United States of America
I found that the local plywood store that mainly supplies cabinet makers to be a good source for melamine and plywood. Since I am not commercial, I come with cash (and call ahead for pricing). They will help load but my purchase is a small drop in the bucket for them and they do not cater to the individual purchaser, but are willing to put up as long as I act nearly professional <grin>
Reply With Quote
  #4  
Old Thu 08 October 2015, 21:19
ger21
Just call me: Ger
 
Detroit, MI
United States of America
I would say that your rpm is too low for a 1/8" bit at that feedrate. It's also very important that you use a sharp bit, especially with lower quality melamine.
Most importantly, do NOT climb cut.
Reply With Quote
  #5  
Old Thu 08 October 2015, 21:42
digger
Just call me: Milosh #113
 
Toronto
Canada
Ger, it may look too low. I used chip load value of 0.014 for 1/8 compression bit as a reference because couldn't find exact value for a regular bit for cutting melamine. Maybe I did cut it a bit more agresive. I should try 120ipm and 10000 rpm. In that case chip load would be 0.06 or even to go with 18000 and same speed. Then I'll make dust. .

Thanks for the info about cutting direction.
Reply With Quote
  #6  
Old Thu 08 October 2015, 21:46
ger21
Just call me: Ger
 
Detroit, MI
United States of America
Just try 15,000 rpm at the 280ipm.

And dust is better than chipped melamine.
Reply With Quote
  #7  
Old Fri 09 October 2015, 06:30
Robert M
Just call me: Robert
 
Lac-Brome, Qc
Canada
Send a message via Yahoo to Robert M Send a message via Skype™ to Robert M
I'm no melamine CNC Gooroo nor experienced many various set-ups strategies, but when I cut cheep melamine, I use a 3/8 compression bit, with a rough cut at +/- 2 to 3x to achieve depth cuts ( +/- 1/4'' to 5/16''), then a finish pass with +/- 0.020 to final size at +/- 200 to 225ipm.
Regardless the quality of the material, a "near" perfect no edge chip every time

In my view ( debatable) so many different possibilities.....since so many machine set up making it many diff. restrain / results !! ....but a roughing pass to then a finishing pass, in my book ( and some modest experiences)....you'll always end up with a nice ( at least nicer) finish...trouble free !
If you need to cut "zillion" boards and must be "super" efficient, then, right....you better find the sweet setup as profit and finish vs productivity make you.....making it or loosing it !

My 2ct.... Cheers
Reply With Quote
  #8  
Old Fri 09 October 2015, 12:45
digger
Just call me: Milosh #113
 
Toronto
Canada
Robert, agree with you 100%. If the time is not constrain, this is the way to go.

Ger, I managed to get way better results. Thing is that I raise speed to max, to 1800, and lower the feed to 60IPM. This improved cutting quality, but the most improvement I've got from changing the bit to new one, to sharp one. Cut line is almost without any chipping. I think, this will be the way to go. I will take a bit more time, but, time is not a problem. So, let it be the dust.

Ger, thanks for good advices.
Reply With Quote
  #9  
Old Fri 09 October 2015, 13:00
ger21
Just call me: Ger
 
Detroit, MI
United States of America
Run the feedrate as high as you can without chipping, and your tools will last longer.
Reply With Quote
  #10  
Old Fri 09 October 2015, 13:24
Robert M
Just call me: Robert
 
Lac-Brome, Qc
Canada
Send a message via Yahoo to Robert M Send a message via Skype™ to Robert M
Very true Gerry....and would not debate this tried & true point you stated.

but, many time I'm ( and other too) are facing some restrain either with the materiel or time wise....or worst, the customer bring the mat ( EI....your commissioned to only finish the dimension with some "special" shape, as the customer brought the rough cut part) !!!
Anyway...
If it's a little series or worst, a "one of".....can't "waist" time neither risking going....a tab faster.....only to see it was just that little to fast.
I rather take the "safe & slower" approach.....end result, clean, satisfied client... and profit !!
Tool wise, your more then right here again....but !!...cost on end mills is small vs retake a "oups".....or better yet, I get my mills resharpened for less +/- 15 per.....and charge accordingly the commissioned pieces for its proportion....if not all.
With all respect....
Reply With Quote
  #11  
Old Fri 09 October 2015, 14:21
digger
Just call me: Milosh #113
 
Toronto
Canada
Robert, when you cut rough melamine with 3/8 compression, is your speed also 200-220ipm?

Ger, a bit of a digression of the subject. What is the limmiting factor of spindle's rpm? Is it bearing speed or there is something else?

Thanks
Reply With Quote
  #12  
Old Fri 09 October 2015, 15:20
ger21
Just call me: Ger
 
Detroit, MI
United States of America
Spindle speed is dictated by the design of the spindle, which I believe has to do with how the motor is wound? You can't go any faster than the spindle was designed to go.
But yes, bearings are also a factor. With higher end router spindles like HSD, ceramic bearings are usually used for 24,000 rpm spindles.

Fwiw, on an industrial machine, I cut melamine with a 3/8" compression spiral at about 800ipm and 17,000 rpm. With a 3 flute 1/2" compression bit, I cut at about 1200ipm and 15,000 rpm. With a good quality bit, I can get over 100 sheets of parts out of 1 bit before the edges start to chip.
Reply With Quote
  #13  
Old Fri 09 October 2015, 16:21
danilom
Just call me: Danilo #64
 
Novi Sad
Serbia
Also if you cut in multiple passes a material like melamine tends to wear the edge of an endmill where it cuts the melamine, so vary the depth a little bit after each use to avoid the damaged (worn not sharp any more) segment doing the cutting of melamine layer.
Reply With Quote
  #14  
Old Sat 10 October 2015, 15:44
Andrew_standen
Just call me: Andrew #109
 
Dorset
United Kingdom
I had all sorts of problems cutting melamine at work. All went well for four or five sheets then chipping started as the cutter dulled. We used 5 cutters a month...at 35 pounds a cutter....Tried many many many different solutions . Different cutters. Feeds speeds. Then i had a 5mm dia pcd.made for us. Cost 130 pound .We run this new cutter at 16000 rpm feed 350mm doc 5mm. Sounds slow I know. But we have cut over 400 sheets on this one cutter over the last year and it's as sharp as when we started. No chipping at all. We cut 20 or 30 parts on one sheet of 13 mm double faced melamine marine ply. Best money we spent best cutter...ok cost a lot but....i test cutters for work on my mechmate. .Cheers Andrew

Last edited by Andrew_standen; Sat 10 October 2015 at 15:53.. Reason: missed an important part doc out...oops
Reply With Quote
  #15  
Old Sat 10 October 2015, 16:54
ger21
Just call me: Ger
 
Detroit, MI
United States of America
Quote:
We cut 20 or 30 parts on one sheet of 13 mm double faced melamine marine ply
I would say that the plywood core was the likely cause of your problems.
Reply With Quote
  #16  
Old Sat 10 October 2015, 17:06
servant74
Just call me: Jack
 
Nashville (Tennessee)
United States of America
In the US, Amana Tools makes poly crystaline diamond router bits. Available through various sellers, including Amazon and Tool City.

They cost a lot more ( 10x or more than tool steel ), but they last a very long time. I know one guy that cuts a lot of MDF and swears by diamond bits.

I just assume melamine wouldn't be to much different for this kind of bit.
Reply With Quote
  #17  
Old Mon 12 October 2015, 08:00
Andrew_standen
Just call me: Andrew #109
 
Dorset
United Kingdom
We use Amana tools quite a lot. We cut all our Mdf and Tricoya with pcd's. They work well.
We also use a lot of Leitz tools.
just wanted to say if you are having problems with laminate use a pcd tool
we cut all our plywood with different tools. Some pcd some solid carbide. Single flute and double both compression.
We must go through 40 sheets a day and have done for the last 8 years
Reply With Quote
Reply

Register Options Profile Last 1 | 3 | 7 Days Search Today's Posts Mark Forums Read

Thread Tools

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -6. The time now is 00:27.


Powered by vBulletin® Version 3.8.3
Copyright ©2000 - 2018, Jelsoft Enterprises Ltd.