Hello Guest it is October 22, 2019, 06:47:30 PM

Author Topic: Feed Rate All Over the Board Question  (Read 1776 times)

0 Members and 1 Guest are viewing this topic.

Feed Rate All Over the Board Question
« on: October 30, 2017, 04:45:57 PM »
Hi...Depending on what or who I listen to or calculation I use...To Cut in to Soft Brass ...Higher Lead Content...

I get Feed Rates from anywhere between 4 and 15...

in Inches...I am using a .010 Engrave bit...40 degree angle...1 cutter.. 1/8" x 2".....Max Spindle RPM is 8000...

Would Like to cut at a Depth of  .02"....Still Trying to learn....but I get Feed Rates of ...4.....9.2......and 15......Depending on who's website and formulas I use....

Thank you
Billy
Re: Feed Rate All Over the Board Question
« Reply #1 on: October 31, 2017, 03:25:39 AM »
Hi Billy,
I don't do much engraving but do use a lot of really small endmills. I agree depending on where you look or read there is a wide range of feeds and speeds.

One thing which I have noted is that the surface speed for a given material and a given tool and surface treatment is consistent across a number of published
sources. With softer materials like aluminium and brass the speeds are quite high and considerable latitude can be taken. Try the same with mild steel, it won't work,
try it with a medium to high tensile steel, or even worse, an austenitic stainless steel and your tool briefly glows red before breaking!

When I started I thought (wrongly) that because I had a high speed low torque spindle that I would spin small diameter tools fast with very low chip loads when
cutting steel, it didn't even come close to working! In the end I had to make a high torque spindle, or at least high torque relative to the size of my machine, 6Nm,
and I'm running direct coupled so max rpm is only 3500. It makes mincemeat of steel, even tough stuff like stainless.

I think your application will require you run at max rpm, 8000 is hardly earth shaking. I would be tempted to run at the high end of the feed range. If you go too fast
the tool life will suffer and any upset will cause breakage. A bit less than that and you'll get good productivity and fair toolife. You can slow the feed down even more
and while the tool life might be good it will have to be  as it will take an age to cut anything. If the feed rate is too low all you end up doing is giving the material
'a damn good rub' which workhardens the material, heats the tool and achieves piss all.

A lot of sources suggest that carbide shouldn't be run cooled, I find that flood cooling, as much as I can get in fact, gives me best results. In part its due to chip clearance,
nothing promotes wear, heat and edge build up like re-cutting chips. Flood cooling helps bigtime with toollife and cut quality.

When I cut heavy copper circuit boards (the copper is 0.42mm thick!) I use 0.5mm 2 flute carbide uncoated endmills at 24000 rpm with  as much cooling flow as I can
squirt at it.  I cut through the copper in one pass and a little bit into the fibreglass underneath, a cut of 0.45mm depth with a 0.1mm stepover at 400mm/min.
When plunging or slotting when taking the first cut I cut to depth in two passes, 0.225mm then 0.45mm at 24000 rpm and half speed feed ie 200 mm/min.

As you can see I have worked these figures out for myself, while I have a published surface speed of 250m/min for copper I have over a period of time refined
that number depending on other cut parameters. One of the early realisations I had was that it doesn't make sense to make a lot of really shallow cuts, it wears
just the very tip of the tool and takes forever to do a job. Now I like to make my tools work for a living about 75% of max and at feed rates that give a decent chip.
Any poor choice or control of your toolpath is likely to result in a broken tool but I'm now getting about 4 hours per tool on the heavy copper boards. When I started
I couldn't get more than 1/4 hour and achieve damn-all in that 1/4 hour to boot!

My suggestion is experiment some. Record the critical parameters, not the rpm or feedrate, but surface speed and chip load. These two are the really useful ones
that will allow you to extrapolate to find new cutting solutions.

Craig
My wife left with my best friend...
     and I miss him!
Re: Feed Rate All Over the Board Question
« Reply #2 on: October 31, 2017, 04:11:08 AM »
Hi Billy
the calculations are:

0.5mm diameter x Pi=1.57mm circumference
1.57 x 24000=37700 mm/min=37.7 m/min surface speed, a long long way short of 250 m/min recommended for copper, but as fast as my spindle will go.

With small diameter tools chip loads of between 1-2% of diameter are indicated. A 1/4 inch endmill can tolerate 3-8% of diameter being that much stronger.

2% x 0.5mm diameter = 0.01mm (10um) per tooth per rev.
2 (flutes) x 0.01mm x 24000=480mm/min

So a feed rate of 480 mm/min results in a 2% of diameter chip, I usually back it off a little...to in this case 400mm/min.

Engagement= 0.45 (depth of cut) x0.1 (width of cut) / 0.5x0.5 (diameter squared)=0.18 or 18% Engagement ratios of 10-30% are common with small tools
but with larger tools 50-100% are possible.

When plunging and slotting:
0.225 (depth of cut) x 0.5 (width of cut) / 0.5 x0.5=0.25 or 25%  Note that plunging and slotting are by far and away the hardest of cutting ops and while the
engagement ratio is in the zone I slow the feed to accommodate the difficulty of the cut. The main problem is chip clearance, this is where flood cooling
helps. At some future date I hope to have some high pressure coolant nozzles to assist with chip clearance when plunging or slotting. As it is I slow the feed to half
of normal chip load ie 200 mm/min.

Craig
My wife left with my best friend...
     and I miss him!
Re: Feed Rate All Over the Board Question
« Reply #3 on: October 31, 2017, 06:17:25 AM »
Thank you...Give me some food for thought....Much appreciated...you did a lot of research ! ! !
Re: Feed Rate All Over the Board Question
« Reply #4 on: October 31, 2017, 09:59:47 AM »
Still coming up with crazy numbers....but not giving up
Re: Feed Rate All Over the Board Question
« Reply #5 on: October 31, 2017, 01:57:06 PM »
Hi,
there is no one set of magic numbers, especially for these small tools and particularly engraving tools when its hard to define a diameter.

My experience suggests that chip load is the most significant number. It really is an estimate of the strength of the tool. 2% of diameter per cutting tooth
per revolution is a good place to start.

Craig
My wife left with my best friend...
     and I miss him!
Re: Feed Rate All Over the Board Question
« Reply #6 on: October 31, 2017, 02:19:22 PM »
I think I will start with the 9 Feed Rate...Plunge 4 and take it from there.... 8000 RPM...Cut Depth at ..03mm and a second pass at .06mm so 2 cuts at .03mm....Take it from there...For the Soft Brass....As for the Plastic...Its Cutting Great ! !

Billy
Re: Feed Rate All Over the Board Question
« Reply #7 on: October 31, 2017, 03:26:37 PM »
Hi Billy,
what is the chip load at those settings?

Craig
My wife left with my best friend...
     and I miss him!
Re: Feed Rate All Over the Board Question
« Reply #8 on: October 31, 2017, 04:04:55 PM »
I get .04mm or .01"
Re: Feed Rate All Over the Board Question
« Reply #9 on: October 31, 2017, 05:31:35 PM »
Hi Billy,
i suspect you are right near the strength limit of the tool. 0.01 inch chip / 0.01 inch diameter means 100% chip load.
Given that it has a single edge means it probably stronger than my two flute endmills say. More cutting edges means
lower chip loads for a given feed and speed.

Craig
My wife left with my best friend...
     and I miss him!