Speed and feed question

[Brian RutherfordParticipant @brianrutherford79058]

I have to cut two semi circles out of 15mm hot rolled steel plate on my toolco 32 mill (similar to WM 18). Semi circles are 30 and 40mm radius. My mill has been converted to cnc. I am using a circular toolpath and a 6mm carbide slot drill 2 flute cutter. What spindle speed and feed rate should I be using. It's tough stuff.

[Brian RutherfordParticipant @brianrutherford79058]

[EmgeeParticipant @emgee]

Brian

Whatever speed and feedrate you use it will be best to have flood colant or a good air blast going to keep the chips out of the slot you are cutting, you don't say if you are leaving tabs but it may be a good idea.

Emgee

[Anonymous]

I'd be running 2500rpm and around 250mm/min. Flood coolant is essential.

Andrew

[Brian RutherfordParticipant @brianrutherford79058]

I cut the first semi circle out with spindle speed set at 2000rpm. The feed was 120 mm per min. Used compressed air to cool the cut. The tool is only cutting 50% of the time as half the circle is outside the cutting area. I ask the question because the machine really struggled . Depth of cut was only 0.5mm. I didn't care to go deeper or faster feed. Motor only goes to 2200rpm.

[Brian RutherfordParticipant @brianrutherford79058]

I cut the first semi circle out with spindle speed set at 2000rpm. The feed was 120 mm per min. Used compressed air to cool the cut. The tool is only cutting 50% of the time as half the circle is outside the cutting area. I ask the question because the machine really struggled . Depth of cut was only 0.5mm. I didn't care to go deeper or faster feed. Motor only goes to 2200rpm.

[Brian RutherfordParticipant @brianrutherford79058]

Emgee, left 2 tabs save the lump falling into the cutter. I do have coolant but the tank is full of paraffin as I mostly cut aluminium. I think I might need to get a small amount of coolant for these occasions. Had no problems cutting steel in the past but mostly en1a. .

[Andy AshParticipant @andyash24902]

I have a cheap Chinese mill, it's the next size down from yours, and mine was made badly…. In a bad part of China.

You might get away with more than I do, but I don't think I would even bother trying to hog this out of plate. I have ended up upgrading a stent cutter grinder so I can keep my cutters razor sharp. I get away with a lot more since I did that. I try to use the biggest cutter I can, to maximise tooth life. I have modified the mill so it can go fairly slowly and still have grunt.

In your situation with my machine, I'd have the blanks laser cut and finish them on the mill as option one. Second option would be to make a disposable MDF template and use the plasma cutter to burn them out of plate, before finishing them on the mill.

[JasonBModerator @jasonb]

I'd approach it differently and be using an adaptive tool path so using the side of the tool not just the end and cutting 5.2mm vertically ( 15/3 plus a bit of breakthrough) and 0.6mm horizontal DOC. Speed 5000 rpm and feed of 4-500mm/min.For a 3 flute cutter Leave 0.3mm for a couple of finish passes 0.2 and 0.1 at same rates. Cut dry.

Video of me trying a few feed rates on EN3, settled for what I list above. I would use the same on hot rolled but pickle it first to remove the scale.

 

 

Not sure what your top speed is so you may have to reduce my numbers eg if top end is 2500rpm then use that and 250mm feed for 3-flute or 160mm for 2-flute. These are for the adaptive, run 75% of that if using full width of tool

 

Even if you want to use the same tool path that you have then you don't really need to use a 2-flute cutter as it is not as though you want an exact size slot. better a 3 or even 4 flute then feed rate can be increased for the same chip load and if you make the final pass at finished profile then the these cutters are better suited to that than a 2-flute.

 

Edited By JasonB on 14/02/2022 07:18:14

Edited By JasonB on 14/02/2022 07:21:51

[Brian RutherfordParticipant @brianrutherford79058]

Thanks Jason,

My top speed is only 2200rpm. Pro rata my feeds are not that much less than yours as it's a 2 flute drill. I used a circular toolpath so it doesn't have to cut all the material away. The plates are for mounting a water cooled spindle. The original motors are not designed for continual running flat out for long periods

[Anonymous]

Just had a look at another job I did machining lever blanks from hot rolled steel plate with a 6mm 3-flute uncoated carbide cutter. I was running 3800rpm and 200mm/min with full width cut and 2.05mm stepdown.

Andrew

[Brian RutherfordParticipant @brianrutherford79058]

Thanks Andrew, again running at 120 mm and 2000rpm full width of tool not much different to you. Step down is a lot less though

[Brian RutherfordParticipant @brianrutherford79058]

Thanks Andrew, again running at 120 mm and 2000rpm full width of tool not much different to you. Step down is a lot less though

[Howard LewisParticipant @howardlewis46836]

For a Slot Drill your feed should be 0.002" (0.050 mm) per rev

So at 2500 rpm the feed rate would be 25 mm per minute with a HSS.cutter, 100 mm for a carbide cutter

With a 6 mm carbide cutter you could probably run faster than 2500 rpm., and increase the feed to match.

Howard

[Anonymous]

Posted by Brian Rutherford on 14/02/2022 10:23:49:

….Step down is a lot less though

Not sure why that should be. For reference my hobby CNC mill has a 1.5hp induction motor driven by a VFD. At the speeds mentioned the VFD is running in constant power. With the speeds and feeds mentioned the mill certainly didn't sound laboured.

My CNC mill has the same horsepower as my Bridgeport. While the Bridgeport will happily drive a 1" diameter endmill I've learnt that the CNC mill is far happier running small cutters at high spindle speeds and feedrates. For general work I use 6mm and 10mm 3-flute cutters on the CNC mill.

Andrew

[Nigel McBurney 1Participant @nigelmcburney1]

Have a bit of sympathy for your Mill ,why put such a load on a relatively small machine,hot rolled plate is for fabrication not machining,quality of this material varies ,and if I do have to deal with black hot rolled steel I use my Colchester as first choice, its easier to turn hot rolled rather than mill.

[Brian RutherfordParticipant @brianrutherford79058]

Nigel I totally agree. I used it for cheapness. It's been a pig to machine but lesson learnt

[Anonymous]

Posted by Brian Rutherford on 14/02/2022 15:32:35:

…been a pig to machine…

It can be a bit gummy. But if speeds and feeds are in the right ballpark it machines reasonably well. I use a lot of hot rolled rectangular section, for the following reasons:

1. I've got a lot of it, as it is cheaper to buy standard 6m lengths than just the amount needed

2. It's less likely to distort than cold drawn when machined

3. It seems less prone to rust compared to EN1A

4. It is easy to weld

Andrew

[JasonBModerator @jasonb]

One problem with your very shallow 0.5mm cut is that the first pass with be removing the scale and that can be quite abrasive, subsequent passes will just be using that same blunted 0.5mm of cutter end.

Was it a new cutter or had it been used for similar shallow cuts before and what about it's parentage?

I don't mind a bit of hot rolled and do use it on my fabricated engines where the bit of texture on the surface is an advantage when replicating cast parts.

[Brian RutherfordParticipant @brianrutherford79058]

I used an old cutter to get through the surface then terminated the program. Then ran it again with a newish cutter. Cutter was a cheap one though. The other reason why I used hot rolled steel was I wanted the finished job like a casting which I will paint to match the machine.

[Author]

Posts