Sharp Corner Problem

[dempseyrob]

Hi all, I hope this finds you well.

Cutting out shaker style doors & drawer fronts today and I noticed 4 different patterns on the outer corner. Inner corners also have a similar effect but can be chiselled out easily. Any tips on what's happening here?

Photo attached, it is taken from the side of the machine (up/down on the image is the X axis, left/right is the Y)

No noticeable sound that would cause alarm, nor is there any odd shaking / jerking.

Setting is to roll around the outer corner. No settings for inner corner, '2D Pocket' operation.


Avid CNC 48 x 96, 4HP spin
Fusion 360
6mm compression bit on 22mm MR MDF
Feedrate 6000 mm/min, Lead In 3000 mm/min
3mm maximum step-down


Many thanks.

Similar Threads:

• I need to mill some sharp corner using an 60 degree chamfering endmill, any advices ?
• Problem- No sharp corner
• Problem- Sharp corner lettering
• How to make a sharp corner on a mill?
• Making a sharp inside corner?

[peteeng]

Hi Dempsey - What's the spindle speed and what tolerance did you set in Fusion? Did you model the groove (if so is it 6mm wide?) or did you sketch a path? Peter

[dempseyrob]

Hi Peter,

15,000 rpm and it's a '2D Contour' operation my apologies, I'll correct it above if I can.

Tolerance 0.01, Roll around corner.

The doors are modelled in Fusion and the contour selected is the bottom outer edge of the door. So it's not a 6mm groove.


Rob

[peteeng]

Hi Dempsey - Does this show in the simulation? Have a close look and I assume the compression bit is 2 flute? Peter

[dempseyrob]

Hi Peter,

The simulation shows the tool rolling around the corner, lifting and plunging for another pass. It doesn't show the tool eating into the doors.

The other noticeable thing is that the wavy move is consistent on each pass. I've also noticed it on an inner corner on a separate operation.

Screenshot attached of the simulation.

2 flute - yes


Rob

[peteeng]

Hi Demp- Just did a square in fusion with your settings and Fusion is OK. So I expect it is something to do with your controller settings on deceleration. Going from 6000mm/min to stop is a bit of a brake. The 6m/min-15000rpm and 2F give you a chipload of 0.2mm/rev. This can be seen in the tool dialogue box. This is a medium cut 2% of diameter is light 4% is heavy so your midrange. 6x0.034=0.2. maybe run the spindle a bit faster to lighten the cut. But I don't think that's your real issue. If the code is straight and the tool is wobbling then the machine is not rigid enough at that setting to achieve the cut. Either the tool load is pushing the tool aside (so lighten the chip load) say to 0.15mm/rev even 0.1mm or the deceleration is set too high and the machine is resonating as it decels and cuts. Either way you need to look at the configuration of the settings. There is also an overshoot so look at the settings to see what the controller is set ay and tighten the settings up or just reduce the accel maybe so its a softer decel. Peter

CL=feed/(RPMxN)

feed mm/min
rpm = rpm
N = no of teeth

run the spindle at full tilt so it has full torque and figure out the feed to get your correct CL say 0.1mm, But in the mid cut area where the velocity is 6m/mm the cut is good, its in the decel zone that's its poor. say its halfway thru the decel zone so its doing 3000mm/min then the CL=0.4mm (nearly a 7% chip on dia) and that's a big chip... so it pushes the tool aside if the machine is not stiff enough. Your tool supplier will have a chip thickness/rev chart for the tool...

some programmers put a small rad in this sort of corner say 0.25mm. Then the decel is not quite as bad, depends on how your velocity planner handles this sort of thing. Again look at your controller settings and figure out how it looks ahead, how it handles 90degs and small rads...

Is it only wavy on climbing cuts? A heavy cut tends to chomp in or down cutting as well? Is the overshoot programmed? It looks intentional?

[dempseyrob]

Hi Peter,

You're a gentleman, thank you.

I understand what you mean with all of that, I've had a cursory look at chip load and decel range so its about time I went in a little deeper.

If I may check in again I might share the Mach 4 configuration settings if I'm having trouble?

Many thanks again,


Rob

[peteeng]

Hi Rob - I assumed the wobble was on the decel side but is this correct? It makes more sense if its on the exit side, climbing and accelerating? So your spindle has enough HP to make the cut but the machine is not stiff enough to hold the line at those settings. have to back something down a bit... Also the 3mm DOC is light so if you slow down to reduce loads to say 3000mm/min you can go to 6mm DOC to maintain the same cycle time if that's important to you. eg if your making $$$ and machine has to be fast...Peter

[dempseyrob]

Hi Peter,

The toolpath is going clockwise around the doors, so you're right the wobble is on the acceleration.

The machine is due a check over, I wouldn't swear that it is stiff enough at the moment. I'll do that first and see how the next one comes out.

Thanks for the tip on DOC, I'm happy to get the finish right first before ramping up and it's not a noticeable issue from a client's perspective.


Rob

[peteeng]

Hi Rob - It can be counter intuitive, but a deeper DOC puts less stress on the tool and you improve tool life. The wobble maybe also clearance in the Z axis. So have a quick check over that everything mechanical is snug and tight. If you do light DOCs you wearout the end of the tool and miss out on all the tools life. The deeper the DOC the less leverage on the spindle there is, so less tool deflection which again helps life. As long as the chip thickness is correct and the tool can clear the chip then go as deep as possible, even full sheet depth. If you have an auto tool changer then a 1F tool for roughing can be run really fast and deep then do a finish cut. Peter