MechMate CNC Router Forum

MechMate CNC Router Forum (http://www.mechmate.com/forums/index.php)
-   Cutting various materials - bit selection, feeds, speeds (http://www.mechmate.com/forums/forumdisplay.php?f=82)
-   -   Cutting Nylon (http://www.mechmate.com/forums/showthread.php?t=1612)

Farproducts Tue 07 April 2009 06:15

Cutting Nylon
 
Good afternnon people,

Can anyone help me with the rpm's and feed rate on cutting Nylons? I am using Belin bits and would like to get some help from someone with experience cutting Nylon.

Thanks!

Conrad

Rad Racer Wed 15 April 2009 14:02

Conrad,

Although I do not have direct experience cutting nylon.....I know the downloadable Onsrud catalog, has feedrate and chipload information tables. Perhaps these tables will help get you started.

www.onsrud.com

KenC Wed 22 June 2011 05:16

1 Attachment(s)
Hello,
I tried to engrave some diamond v-grooves on nylon & this is what I end up with...
Attachment 11933

Tried various feed rate & spindle speed combination but results isn't satisfactory.
3800rpm to 19000rpm & 2800 to 5600mm/min without improvement.

Would most appreciate if anyone could point me the right direction.

bradm Wed 22 June 2011 05:43

I've never tried to do that, but looking at your picture, it appears that you're getting okay cuts, but the chips aren't quite releasing.

That strikes me as more of a bit geometry / sharpness issue that a speed and feed one. Dumb ideas:

- Cut it twice; second time go the other way ( climb / conventional or conventional / climb ).

- If those chips are all attached at the top surface, how about belt sanding it (or skim cutting with a square edges bit) to release the chips?

KenC Wed 22 June 2011 06:24

It look & feels like a very rought carpet :p My client say it makes great anti slip flooring...:(
I did swap bits, cut it multiple times but the results were the same....
Tried sanding paper but after 2 strokes, I know that is a bad idea. Even filing is not the solution...
Tried googling, most people apply coolant, & you know we don't let water near our MM :(

smreish Wed 22 June 2011 07:37

Notes from my machining class - a VERY long time ago:

TIPS FOR MACHINING NYLON
STORAGE
Nylon has a high coefficient of thermal expansion (about three times that of aluminum) and low heat conductivity. Make sure that it has been exposed to normal room temperature for several hours before it is machined into finished parts.
SAWING
Nylon can be easily sawed on standard metal working equipment. Wood working equipment may be suitable but the high cutting speeds may cause excessive heat build-up. A blade that has been used for cutting metal is usually not sharp enough for nylon. Use a new coarse tooth blade with good set. Coolant may be used to control heat buildup and to prevent melting the nylon.

HOLDING
Keep in mind that nylon is not as strong as metal and can be deformed by improper chucking methods. On small accurately sized rod, use standard spring collets. On larger parts, use a 6-jaw universal chuck instead of a conventional 3-jaw chuck to distribute the holding force more uniformly. For thin walled tubular shapes, machine soft jaws so that the part is almost entirely confined.

TURNING
Satisfactory finishes can be easily obtained on nylon over a wide range of surface speeds. Use tools that are honed sharp and have high rake and clearance angles, to minimize cutting force and reduce heat build-up. Chips will be continuous and stringy. They should be directed away from the cut and prevented from winding around the workpiece. Coolants are generally not necessary for lathe work unless there is excessive heat build-up.

MILLING
Milling cutters should be honed sharp and should have high positive cutting angles. Care should be used in clamping the part to prevent distortion. Double-faced pressure sensitive tape can be used to hold down flat parts. Cutting speeds and speeds will be determined by the finish required and will be limited by heat build-up.

DRILLING
Use conventional twist drill or flat type drills. Polished flutes will aid in the removal of chips. Do not use metal cutting reamers with nylon. They do not cut freely enough. Drill small holes to size in one operation. Rough drill large holes and finish by single point boring.

THREADING
Use only sharp taps and dies on nylon parts. Don't use tools that have been used to cut metal. H5 or even larger oversized taps may be required because a threaded hole in nylon closes in when the tap is removed. Threads to close tolerances can be easily single point chased.

GRINDING
The large amounts of heat generated by grinding, together with the low heat conductance of nylon, usually dictate that liberal amounts of coolant he used in most grinding operations. Thru-feed centerless grinding of long, flexible parts of nylon can be easily accomplished, and tolerances as close as .0005" are possible. Cylindrical grinding on nylon is usually not required because it is easy to get good finishes and close tolerances on a lathe. Surface grinding of nylon is usually not necessary. If a flat surface with close tolerances and good finish are required, the best approach is fly cutting in a milling machine. No, not cutting a fly on your milling machine, FLY cutting.

STAMPING
Thin pieces may be stamped with standard equipment. Thick sections will require high shear angles if good edges are needed. Steel rule dies may be used for some parts.

MEASURING
Use ordinary measuring equipment. However, use a light touch because the material is not as hard as metal. A micrometer anvil can deform a nylon surface as much as several thousandths. Homemade, soft plug and ring gauges are useful on thin walled parts. If extremely close tolerances are involved, make SURE any temperature changes that the part will see are taken into account.

KenC Wed 22 June 2011 08:02

That is great info. pardon my ignorant, What positive cutting angle :o...

smreish Wed 22 June 2011 08:11

= climb cutting, but conventional cutting may work too. But in this context, I think they mean a cutter with a rake more that 45 degree (which is higher than 50% of the available cutting angle)

Please, others that have better information, chime in here....I haven't dealt with this in years.

Sean

KenC Wed 22 June 2011 08:18

If cutting angle=rake angle, it makes sense to, I just looked at the V-bit & it has negative rake angle.
BUT, I'll just try climb cut & see what happens.

KenC Wed 22 June 2011 08:37

1 Attachment(s)
Climb cut result

Attachment 11935

A lot better but still far from desirable...

KenC Wed 22 June 2011 09:27

1 Attachment(s)
As any drill bit will have a much higher positive rake angle then straight flute router bit. I took a drill bit & re-grind it...

with 3000rpm, 3300mm/min this is what it produced

Attachment 11936

Much better, but still a tat shy from what I hope to achieve.

But its close to mid-night, I can sleep with this result... :D

MetalHead Wed 22 June 2011 15:38

Can you try to run over it with a hand torch to get rid of the burs? I think they do that with acrylic.

KenC Wed 22 June 2011 22:13

I'll try to borrow, steal or rob a torch to try it out. Will show the result when I'm done with it.
Anyway, the client was pleased with the finishing, now all we need is his boss to approve the purchase order...
Thanks Sean, couldn't had done it without you.

ciao

Gerald D Wed 22 June 2011 23:40

If it will be a big order then I would consider a special toolhead motor and cutter. Cutter rotation axis horizontal (maybe the small angle grinder again)......

mikefoged Thu 23 June 2011 06:45

I use air to cool and to get the chips away this is importent, for bits I use the same that I use for alu. but again they need to be sharp.


All times are GMT -6. The time now is 05:46.

Powered by vBulletin® Version 3.8.3
Copyright ©2000 - 2024, Jelsoft Enterprises Ltd.