Joe's 1000x600x200 steel and aluminium router started

[devmonkey]

It improves somewhat with slower feed, the flute is longer than the material is deep. I just found one source of the problem the bolts holding the Y axis plate that ties the Z to the Y ballnut were not cranked down, they had worked themselves to just loose, nust have forgotton to loctite those one...

Anyway this tidied up the top diameters which are now spot on again, but with the 4mm bit the hole bottom is still smaller than the top, error is much less, maybe 0.05mm. This is enough to be annoying as you get a decent H8 fit to the shaft on one side and but tight on the other, opening up the hole doesn't solve the problem as it becomes loose on the top. Doesn't matter at all for normal profile work just shaft and bearing fits. I will stick with the 6mm known quality cutters for doing these.

I also just ordered a hopefully decent set of collets from Arc, not convinced by the much cheaper set I have based on the damage they take when you break an endmill.

[devmonkey]

I've done some more experiments to try and determine the source of the non-vertical walls I get cutting SRBP with single flute endmills. I surfaced the spoil board and trammed the spindle before running these tests.

In all cases the toolpath was a 25mm square in 10mm material, outer roughing profile to 9mm deep leaving 0.2mm for a single finish path at full depth.

#1 4mm Chinese SF, 0.2mm taper top to bottom,
#2 3.175 Chinese SF, 0.1mm taper top to bottom,
#3 6mm Euro SF, 0.03mm taper top to bottom,
#4 6mm Chinese 2Flute, 0.00 taper top to bottom.

The taper is not constant, rather it bulges towards the bottom where the skirt was left to hold the part for the finish pass.

I think that with this slightly flexible material the single flute cutters when slotting are leaving a slot smaller than the tool diameter, this is then cleaned up on the finish pass but not where the tool is cutting the skirt. The same material squeezing does not occur with 2 flute cutters. Has anyone else experience this with single flutes, I haven't noticed this happening in aluminium.

[JAZZCNC]

I always find single flutes cut undersize. Never been sure it's a deflection or the tool. I always finish with a 2 flute and I also find HSS gives a better surface finish than carbide in aluminum for the finish passes.

I hardly use Single flute cutters anymore. My preferred method is 3 flute carbide rougher leaving 0.4mm then 1x semi-finish pass @0.3mm and a final 0.1mm final finish pass. For work that doesn't need the best surface finish and accuracy I just take the full 0.4mm as a finish pass.

[devmonkey]

I always find single flutes cut undersize. Never been sure it's a deflection or the tool. I always finish with a 2 flute and I also find HSS gives a better surface finish than carbide in aluminum for the finish passes.

I hardly use Single flute cutters anymore. My preferred method is 3 flute carbide rougher leaving 0.4mm then 1x semi-finish pass @0.3mm and a final 0.1mm final finish pass. For work that doesn't need the best surface finish and accuracy I just take the full 0.4mm as a finish pass.

Hi Jazz, what 3 flute rougher do you recommend? I was quite looking forward to making less chips with these 1/8 single flutes but no point if you have to go around with a 6mm 2 flute to clean up,

[JAZZCNC]

Hi Jazz, what 3 flute rougher do you recommend? I was quite looking forward to making less chips with these 1/8 single flutes but no point if you have to go around with a 6mm 2 flute to clean up,

I mostly cut aluminum and use 8mm reduced neck Alu power cutters from cutwell tools, thou recently I've tried the APT version and they seem ok plus good price.

https://www.shop-apt.co.uk/economy-3...-diameter.html

I also tried these and they give a very nice finish, but I've not got enough time on them yet to see how well they last.
https://www.shop-apt.co.uk/3-flute-v...lc-coated.html

[devmonkey]

Those look excellent value thanks. How deep DOC do you go with the rougher in ali?

[JAZZCNC]

Those look excellent value thanks. How deep DOC do you go with the rougher in ali?

It depends on the grade. I mostly use Cast tooling plate and I can take 4mm DOC slot milling with coolant but I often keep it to half that with a bump in feed to save the cutter but run it dry with air. to keep the mess down. Feeds n speeds I tend to play around with depending on the job but they range from 1000mm/min to 1600mm/min. RPM 12K to 20K often around 15k.

I did play around with deeper DOC and the cutters will happily take 100% Dia but my 2.2Kw spindle isn't very keen, there's nothing left for a safety margin and a slight soft spot will stall it.
Side cutting it will happily take 1.5xD and I often cut 20mm plate full pass just dibbling it away 0.30mm, which is roughly the serration depth, hence my 0.4 finish passes. When using i-machining (adaptive) I can really ramp it up and it's crazy fast at full DOC.

[devmonkey]

It depends on the grade. I mostly use Cast tooling plate and I can take 4mm DOC slot milling with coolant but I often keep it to half that with a bump in feed to save the cutter but run it dry with air. to keep the mess down. Feeds n speeds I tend to play around with depending on the job but they range from 1000mm/min to 1600mm/min. RPM 12K to 20K often around 15k.

I did play around with deeper DOC and the cutters will happily take 100% Dia but my 2.2Kw spindle isn't very keen, there's nothing left for a safety margin and a slight soft spot will stall it.
Side cutting it will happily take 1.5xD and I often cut 20mm plate full pass just dibbling it away 0.30mm, which is roughly the serration depth, hence my 0.4 finish passes. When using i-machining (adaptive) I can really ramp it up and it's crazy fast at full DOC.

Right i'll order a couple, sounds excellent. Are you saying you can cut cast plate full depth (20mm) at 1000mm/min using trochoidal/adaptive? I haven't tried anything like that aggressive, I usually cut at 6mm DOC with a 6mm cutter, ~1600mm/min and 1mm stepover into plate with trochoidal.

[JAZZCNC]

Right i'll order a couple, sounds excellent. Are you saying you can cut cast plate full depth (20mm) at 1000mm/min using trochoidal/adaptive? I haven't tried anything like that aggressive, I usually cut at 6mm DOC with a 6mm cutter, ~1600mm/min and 1mm stepover into plate with trochoidal.

No Using i-machining which is Solid-Cam's version of trochoidal I can cut much more aggressively than 1000mm/min at 20mm DOC. i-machining adjusts the feed based on geometry while it's cutting and usually, it's anywhere between 2000-4000mm/min and 14-18000rpm. And that's on the medium setting 4, if I bump up the level to 7 it really rips chips, but it knocks the hell out the machine and spindle so I keep it between 3-4. This usually spits out feeds between 2-3000mm/min, 12000rpm and varies the step over between 0.1 and 0.9mm. See Pic

[szecho]

I have read this thread and I have a question.
I saw you have plates welded on the frame and a washers under the supports.
How did you position the ball screw support (bk/bf) on the frame? By the thickness of the washers you set the screw to be parallel with the rail?