CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
July 22, 2019, 23:53:13 pm


Login with username, password and session length


Pages: [1] 2
  Print  
Author Topic: Milling ferrous metals  (Read 714 times)
Mark81
Wookie
****
Offline Offline

Posts: 271


View Profile
« on: April 15, 2019, 14:31:27 pm »

Hi hope this kind of questions are tolerated here. I subscribed some CNC forums in the past but I didn't receive answers to my questions. Instead here there are a lot of experienced people that kindly help newbies!

This time I have to cut an inner profile from a galvanized iron (hence ferrous metal) of 1.5 mm thick.
I might cut dozens of this objects so I'm going to buy the correct tool to do the job.
To have an idea I need to cut out a rectangle of 100x30 mm into the stock. The corners should be quite sharp so I'm going to use a 3 mm diameter tool (in order to avoid a tool change).

I guess I have to keep the chip load quite small, say 0.02-0.04 mm, but I don't know the behavior of the material. Hence I don't know what kind of tool is recommended (single or multiple flutes) and the acceptable "window" of the working parameters (feedrate, rpm).

Thanks in advance
Logged
Dragonfly
CNC Jedi
*****
Offline Offline

Posts: 2116



View Profile
« Reply #1 on: April 15, 2019, 15:13:03 pm »

Depends on your machine. Almost impossible on a typical CNC router.
Logged
Mark81
Wookie
****
Offline Offline

Posts: 271


View Profile
« Reply #2 on: April 15, 2019, 15:15:37 pm »

Almost impossible on a typical CNC router.

Why?  Shocked Huh
Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3965



View Profile
« Reply #3 on: April 15, 2019, 15:30:35 pm »

Try a typical milling cutter with 3 or 4 flutes then you can tell us if it worked okay and if it was possible on a typical CNC router.
Logged

Made in England
Mark81
Wookie
****
Offline Offline

Posts: 271


View Profile
« Reply #4 on: April 15, 2019, 15:45:38 pm »

Try a typical milling cutter with 3 or 4 flutes then you can tell us if it worked okay and if it was possible on a typical CNC router.

I didn't say "I'm not agree". I just asked "why".
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3610


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #5 on: April 15, 2019, 16:05:10 pm »

Flimsy like noodle. 

Can cut diamond with noddle if noodle long enough and time infinite. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2628



View Profile
« Reply #6 on: April 15, 2019, 17:49:44 pm »

Almost impossible on a typical CNC router.

Why?  Shocked Huh

Because it don't have the mass and rigidity of a milling machine..  Wink
Logged

My 2¢
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2628



View Profile
« Reply #7 on: April 15, 2019, 17:50:32 pm »

Flimsy like noodle. 

Can cut diamond with noddle if noodle long enough and time infinite. 

 Grin Grin Grin
Logged

My 2¢
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5513



View Profile WWW
« Reply #8 on: April 15, 2019, 18:10:11 pm »

Hello

Quote
I guess I have to keep the chip load quite small, say 0.02-0.04 mm, but I don't know the behavior of the material. Hence I don't know what kind of tool is recommended (single or multiple flutes) and the acceptable "window" of the working parameters (feedrate, rpm).

You can refer to this document for small tools.

http://www.sorotec.de/webshop/Datenblaetter/fraeser/schnittwerte_1_8_en.pdf

so for a carbide tool Ø3 - 2 flutes

cut speed = 90 m/min ; Fz = 0.01 > RPM = 9540 , Feedrate = 190 mm/min

with a small machine, you can try 0.2 mm for depth increment. Use coolant and use a tool as short as possible (and of course a tool designed to cut steel)

I don't know what is your machine, but a router can cut steel ... it's depending of the router.

Here on a BZT PFE 500 PX (the mine but with the previous user) certainly the vice is a little too small !
(DI ~ 1mm)

https://www.youtube.com/watch?v=wVnMlVg383I

++
David
Logged
Garyhlucas
CNC Jedi
*****
Offline Offline

Posts: 1247


View Profile
« Reply #9 on: April 15, 2019, 18:54:36 pm »

Use a four flute coated carbide endmill and plunge in slowly. I’d use a tangent entry into the scrap because on plunge the tool will walk around. When profiling don’t use a climb cut as the flex of the machine may allow the cutter to pull into the material and break it.

My machine is kind of a wet noodle to but I cut steel and stainless with small cutters all the time.
Logged

Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/
dwc
CNC Jedi
*****
Offline Offline

Posts: 534



View Profile WWW
« Reply #10 on: April 15, 2019, 19:06:31 pm »

You can probably find parameters to cut without breaking the tool, but if your machine is not stiff and you cut hard material
you need to expect that the resulting dimensions will need tweeking until they are right.
Circles may not be round etc.
That is from the flexing of the machine, more in certain directions, less in others.
D
Logged

lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7914



View Profile
« Reply #11 on: April 15, 2019, 19:27:59 pm »

Gary,
I still don't understand your reference to 'climb'.  Climb pushes the cutter AWAY from the surface being cut, not pulling into it.

That's why - at proper feeds and speeds - climb will produce a more-accurate and smoother cut than conventional.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2628



View Profile
« Reply #12 on: April 15, 2019, 20:01:57 pm »

Climb pushes the cutter AWAY from the surface being cut, not pulling into it.
*************************
Lloyd, in most cases , yes. But if taking aggressive cut it will grab at the end of a cut(edge) and it will damage the cutter and or part. I did that milling titanium, where conventional cut wasn't an option . It ruined brand new 3/4 dia 6fl end mill on beaffy Kearney & Trecker vertical mill..
Logged

My 2¢
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7914



View Profile
« Reply #13 on: April 15, 2019, 20:29:17 pm »

Yeah, well...

In this case, if he takes an 'aggressive' cut, he'll end up deflecting the spindle to such an extent that he'll not get the dimensions he wants.

Metals CAN be cut on router machines with elastic 'play' in the spindle.  They can't be with machines that just have loose spindles.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3965



View Profile
« Reply #14 on: April 15, 2019, 21:56:30 pm »

I'm not a big fan of guessing, you don't get the answer, it's much better to, "give it a go" and then you know for certain.
Logged

Made in England
Pages: [1] 2
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.21 | SMF © 2015, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.182 seconds with 20 queries.

Copyright © 2018 HexRay Ltd. | Sitemap