Milling Structural Steel (S275jr) on a new Hurco VM20i

This is my first post here so I should point out that I am in the UK and that I am a design engineer (production automation machines) who got fed up being let down by local subcontract shops and have bought a new mill and lathe (Hurco VM20i and TM10). I have spent several years making prototype parts on my manual machines using HSS tools and had hoped that the transition would be a little easier than it has been - imagine that!

I have some flame cut profiles that are 2" thick and 10x34" square. They are in a grade S275JR structural steel from a reputable supplier (I can have material certs if I pay a little extra) which has a minimum yield of 275n/mm but could possibly have a UTS of 560n/mm which I think may be a little tougher than A36 in the USA.

I had a real problem getting YG1 V7 solid carbide cutters to work on this stuff using the suggested settings for a low carbon steel and we (myself and the tool sales guy) have settled on treating it as a high strength structural steel (250-650Hb instead of 100-320Hb). This seems to work for milling (faceing and shoulder) but I keep breaking taps!

I have 33 M6 holes and 12 M10 holes. The M6 tap broke on the 15th hole and the M10 on the 10th hole. The M6 tap went on the way in and the M10 on the way out just as it started to reverse. The M6 was tapping 15mm deep and I reduced that to 6mm with a view to hand finishing to depth (not really why I bought the mill but anyway...). The M10 were reduced to 15mm deep in view of the M^ breaking and I was shocked that it broke an M10 tap on the way out.
The taps are both HSSe YG taps - both brand new spiral flute machine taps and the drill was 5mm/M6 and 10.5/M10. It is very frustrating as I thought I hade everything correct but I clearly have something badly wrong. I hope that someone might have experience with structural steel and also be prepared to share any advice they have.

Living in hope,
Mark

Whenever I have any doubts regarding the material I opt for a thread mill. Less prone to surprise breakages, and usually when they do break, the hole can still be salvaged.

In a past life we did a lot of work on structural steel. We always drilled everything with through holes so that it could be tapped with a spiral point tap (usually with a cordless drill). If you must tap, I really recommend a spiral point if possible. Especially in those small sizes.

S275 is very soft mild steel, typically around 120Bn, not much more. In terms of machined components it is pretty much the shite of the shite specified for maximum cheapness. It tends towards being gummy at the best of times, and is likely to be especially so in the HAZ from profiling.

If you're tapping with cutting oil, which kind? If you're tapping with coolant, don't, unless you can rigid tap fast enough to get close to a reasonable surface speed for this material. You need speed to cut a clean chip, otherwise you need lubricity to prevent chip galling, which is most likely what happened when your M10 broke on the retract.

Thanks for the reply Boosted. I can mill threads on the VM but had avoided it as I thought a few holes would be easy to thread with a tap - I think it might be time to revisit that decision.... The prospect of removing the remnants has me full of joy

Thanks Gregormarwick,

I anticipated it would be soft and I only took it as it was all the profiler had in stock (everything else was going to need to come out of a slab (That I bought). Perhaps I should have got a cold rolled flat and had it water jet to shape - nothing like 20-20 hindsight.
As it happened, I did take a file to some of the sharp edges on the bottom after I finished the profile so I could handle it a little easier and the (new, sharp) file scatted over the burr with little effect. I should have taken notice at that point that it was not anywhere near as soft as I was expecting. The tapped holes are on the edge and well under any remnant of the HAZ (I had 5mm left on the profile and it was flash ground after cutting by the supplier.

I did use coolant (which is new within a few weeks and kept at correct concentration by manufacturer specification). I suppose I should modify the program to stop between holes and turn coolant off for tapping so I can spray some Tapping fluid on/in the hole (Ambersil Tucut).
I had the tapping speed at 164rpm with a 1 second dwell time. The retract speed was actually set at 200% by default so retract speed was 328rpm. I will reduce that to match tapping speed as I am not interested in maximum production speed - these are parts for my own machine builds.

Mark

MC-Design said:

Thanks Gregormarwick,

I anticipated it would be soft and I only took it as it was all the profiler had in stock (everything else was going to need to come out of a slab (That I bought). Perhaps I should have got a cold rolled flat and had it water jet to shape - nothing like 20-20 hindsight.
As it happened, I did take a file to some of the sharp edges on the bottom after I finished the profile so I could handle it a little easier and the (new, sharp) file scatted over the burr with little effect. I should have taken notice at that point that it was not anywhere near as soft as I was expecting. The tapped holes are on the edge and well under any remnant of the HAZ (I had 5mm left on the profile and it was flash ground after cutting by the supplier.

I did use coolant (which is new within a few weeks and kept at correct concentration by manufacturer specification). I suppose I should modify the program to stop between holes and turn coolant off for tapping so I can spray some Tapping fluid on/in the hole (Ambersil Tucut).
I had the tapping speed at 164rpm with a 1 second dwell time. The retract speed was actually set at 200% by default so retract speed was 328rpm. I will reduce that to match tapping speed as I am not interested in maximum production speed - these are parts for my own machine builds.

Mark

Click to expand...

If you can't file it, then it's not S275, and all bets are off.

MC-Design said:

Thanks Gregormarwick,

I anticipated it would be soft and I only took it as it was all the profiler had in stock (everything else was going to need to come out of a slab (That I bought). Perhaps I should have got a cold rolled flat and had it water jet to shape - nothing like 20-20 hindsight.
As it happened, I did take a file to some of the sharp edges on the bottom after I finished the profile so I could handle it a little easier and the (new, sharp) file scatted over the burr with little effect. I should have taken notice at that point that it was not anywhere near as soft as I was expecting. The tapped holes are on the edge and well under any remnant of the HAZ (I had 5mm left on the profile and it was flash ground after cutting by the supplier.

I did use coolant (which is new within a few weeks and kept at correct concentration by manufacturer specification). I suppose I should modify the program to stop between holes and turn coolant off for tapping so I can spray some Tapping fluid on/in the hole (Ambersil Tucut).
I had the tapping speed at 164rpm with a 1 second dwell time. The retract speed was actually set at 200% by default so retract speed was 328rpm. I will reduce that to match tapping speed as I am not interested in maximum production speed - these are parts for my own machine builds.

Mark

Click to expand...

That's an awfully slow rpm for either tap, M6 should be 350-550rpm and the M10 200-300rpm.

I wonder what the vendors, those "let down by local subcontract shops"
Had to say about you selection of materials ?

Gregormarwick, I intend to have a closer look at the hardness in the morning - it certainly wasn't "hard" but it was not soft either. I didn't try too hard at the time in case I slipped and hit the bed (on my brand new machine).

Mark

GMC1724,

Yes, I started out with 350rpm on the M6 but dropped it by 50% and reduced the depth after the first tap broke. Thinking I would be smart, I dropped the speed to 164 in the hope of a straightforward end to the job..... not that that has worked to plan.

Mark

Digger Doug,

Not certain I get what you meant but the part is a bed plate for a wire drive - think in terms of a die set and you have something similar I suppose. Typically this is the material used - it is only there to hold everything in the correct place, no wear or moving parts in contact it just needs to be strong.

Mark

If a file skates, definitely try threadmilling. I threadmill harder materials all the time, problem free.

Mhajicek,

I am thinking that might be the sensible solution as it gives me flexibility with odd sized threads. I just never considered it as I have never had a cnc machine before and still think very much conventional manual machines. I also got told that the Hurco is not great with rigid tapping, especially below M6 but that is hearsay and I have no other reference to benchmark it against.

Mark

MC-Design said:

Mhajicek,

I am thinking that might be the sensible solution as it gives me flexibility with odd sized threads. I just never considered it as I have never had a cnc machine before and still think very much conventional manual machines. I also got told that the Hurco is not great with rigid tapping, especially below M6 but that is hearsay and I have no other reference to benchmark it against.

Mark

Click to expand...

I have Hurcos and they rigid tap just fine, albeit not very fast - that said my machines are much bigger than yours with heavy 50 taper spindles, so yours is most likely able to rigid tap much faster than mine. That was the basis for my comment about how fast you were practically able to run the taps.

I'd want to be running a good coated HSSE tap at no less than 25m/min in S275, 15-20m/min if uncoated.

Don't forget to order the thread gauge go/nogo set. With taps you might be able to get away without them, but with threadmilling you need to size it in to fit the gauge.

MC-Design said:

I did use coolant (which is new within a few weeks and kept at correct concentration by manufacturer specification). I suppose I should modify the program to stop between holes and turn coolant off for tapping so I can spray some Tapping fluid on/in the hole (Ambersil Tucut).

Click to expand...

I'd be a little wary of that, the RTD could contaminate your your coolant unless it's the very last op and the part comes out after.

It would be worth contacting your cutting fluid manufacturer and asking them if they have a tapping fluid that won't contaminate your coolant, I've also heard of people just using the cutting fluid neat hand applied for tapping, not something I've tried personally though.

Two things.

Add a M0 and put tapping wax in the holes.

Do a peck tap and it will be fine IMO. Plus you need to go faster. I tap A36 all the time and essentially always do a peck tap. I recently did a fixture with 100 M5 holes and with the peck it was good to go with everyone.

Also if you are not too worried you can easily go with a 5.1mm drill as well as a 10.6mm on the M12. If you are not holding a tolerance on the threads there is room to make the hole bigger.

Just to be different. If the material is actually soft/gummy then form taping can solve a lot of problems. It would be nice to have an actual measured hardness but if the stuff is as variable as A36 that may not help much. A bit of lube can cure all sorts of problems. Wax, ep grease, moly... Depending on tolerances moving one drill size can make loads of difference in torque needed to tap. Still have to solve the retraction breakage; that is really non intuitive. Hope you solve it. :-)

Well, I should start by thanking everyone for their constructive replies. I think I will try and spend some more time here in the future - perhaps I might even be able to offer some help (probably design rather than machining!).

Rather than reply to each post individually I will respond in general if that is ok with everyone. I went back at the stuff with a file and it is soft - I think the file was not making much impression as it was running on the curved burr that had formed on the bottom of the plate. I have the job raised from the bed by about 2" and I was trying to take the edge off at 45 degrees but working towards the bed and didn't fancy damaging the bed or my hands if I slipped. I also tried manual tapping and it turns out a little tufcut helps immensely compared to coolant as was suggested. It also gave an insight to the problem - the tap gets stuck when I try to back out so I think the material is "gummy" and perhaps grabbing the tap or deforming back into the clearance behind the cutting edge when I try to back out. At least I know for certain that it is a problem backing out rather than tapping. I will try some spiral point taps to see if they break the swarf better and I will add a M0 if I think I can get the tap to work. I have also got some thread mills on the way which I hope to try in the morning so I can reply after they have been tried.

Mark

PS. I just discovered what a can of worms this subject is! I thought I had done my research on this site but it never occured to search for breaking taps

Ok, so today I went and tried out the thread mill. I got a 2D full length cutter and ran the machine with 2 pecks at half the pitch (0.75mm). It worked really well at 60m/min and 0.05mm feed and came out just slightly undersize. Rather than mess about adjusting the offset I simply ran a tap down afterwards.

I also discovered that there is one hell of a difference between the YG1 tap and my trusted Guhring taps..... The YG1 will not back out if it has done any cutting, even chasing the milled thread whereas the Guhring power taps easily snap the swarf off and back out easily and predictably with coolant or tapping fluid (makes no difference that I can feel).

All I have to do now is remove the offending bits of M6 and M10 tap which might involve making a spark disintegrator.

Mark