cnc router x axis starting before y axis finished when pocketing ?

[Robin Oakapple]

I'm using Mach3 by the way, top pocket is at 3 metres/minute and the lower one at 2 M/min (approx approx 120/80 ins/minute)



I don't know how to fix this, so any help would be welcome

[JAZZCNC]

You're not giving enough information for anyone to help really.

However, I'll take a stab because I'm pretty sure it's because your acceleration is too low and you are using constant velocity G64 so you are getting corner rounding due to fact Mach is trying to maintain the Constant velocity command but due to physics there's no way it can cut that tight a radius so to get around the corner it cuts across the grass so to speak.

The cure is to up the acceleration in motor tuning or change to exact stop mode, but this could give you a jerky movement dependant on how the code is generated.! Playing with constant velocity angle settings will also help.

To get the higher acceleration you may need to lower velocity in motor tuning otherwise you could get missed steps. You can't have both high.

[Robin Oakapple]

Thanks for the detailed reply Jazz. I'll certainly have a look at those settings. At my current point on the learning curve, it's difficult for me to know what information would help people help me.

I'm going to guess that velocity in this context is not the same as feed rate? But that's a guess because having set the feed rate differently for the two pockets in the picture there's a difference between them.

[JAZZCNC]

Thanks for the detailed reply Jazz. I'll certainly have a look at those settings. At my current point on the learning curve, it's difficult for me to know what information would help people help me.

I'm going to guess that velocity in this context is not the same as feed rate? But that's a guess because having set the feed rate differently for the two pockets in the picture there's a difference between them.

Details like cutting parameters, so, feed rate, DOC, tool size, etc along with machine parameters so Max velocity and acceleration the machine is set to. Even the size of the pocket and radius on corners etc would help because in the picture there is nothing to judge the scale from. Those radii could be 5mm or 50mm and that would make a big difference.

Velocity and feed rate are the same things the only difference being you have MACHINE (Rapid speeds) velocity and FEED velocity. With RAPID velocity being the MAX machine is tuned to travel at and yes I was referring to MACHINE velocity.
When you tune a machine you can tune it either with a high velocity with low acceleration or high acceleration and lower velocity. But like I said in other posts if you try to tune for both high you run the risk of stalled motors and missed steps.

The motor tuning can make a massive difference to cycle times on jobs. For instance, if you cut lots of jobs with short moves like engraving or 3D work then a machine set up for velocity will actually take much longer to cut the job than one set up for acceleration. Why when the velocity is set high and with a high reedrate.?
Again it's down to the laws of physics, each of the short moves as to accelerate to commanded reed rate and then slow down to blend into the next short move all within a set time period, this repeated for each of the short segments.
Now what actually happens is that it accelerates for a time period but never actually hits the commanded reed rate before it as to start slowing down for the next move. How high the feed rate gets is dependant on how fast the acceleration is set. Think of it like driving a super-fast car between traffic lights spaced close together, the cars top speed is 200MPH but you only ever hit 30mph before having to hit the brakes.

Now in your case, you have commanded 3000mm/Min but you have a low acceleration setup, to compound this the CAM software as probably created G-code that breaks the Arc of the radius corner into short line segments. So Mach3 or the motion planner inside mach3 sees these short line segments and says to the motors NOWAY boys can we stop n start at each of those short line segments but the fact you have commanded G64 or Mach3 is setup constant velocity mode means it must maintain the velocity so it tries but at the last minute says NOPE we've run out of breaks so cut the corner boys else we'll break the constant velocity rule.

So setting a higher acceleration in motor tuning, even of this means lowering velocity will actually allow higher corner speeds in tight corners because it's like giving the car stronger breaks so it can break later into the corner and get around it faster and closer to the path it should follow.
Also to help with getting around the corner fast mach3 provides some extra features for constant velocity(CV) which will actually turn OFF CV on angles above the setting you enter, so if the angle is greater than say 90deg you can have it disable CV then switch it back on. It does this by looking ahead and reading the G-code before the move actually happens, this is why CV and LOOK AHEAD are closely related. They work together but if one is too great other areas may suffer.

For this reason, it's best to start with tuning the motors for acceleration and then play with CV settings and LOOK AHEAD to fine-tune if needed.

One tip is to create profiles with different motor tuning parameters for both high acceleration and high velocity then load the profile which suits the type of work your doing.

[Robin Oakapple]

Details like cutting parameters...

Thanks for the extraordinarily detailed response Jazz, it's very helpful and has given me much to study and experiment with.

By the way, the pockets in the pictures are 150mm by 30mm, 3mm deep and cut with a 6mm compression bit from the Cutter Shop in Fareham. The Gcode was generated in Vectric Cut 2DPro and run by Mach3 to my 1220 x 850 (with 2.2Kw spindle) router which was made by RNR Designs in Stockport.

[JAZZCNC]

Thanks for the extraordinarily detailed response Jazz, it's very helpful and has given me much to study and experiment with.

By the way, the pockets in the pictures are 150mm by 30mm, 3mm deep and cut with a 6mm compression bit from the Cutter Shop in Fareham. The Gcode was generated in Vectric Cut 2DPro and run by Mach3 to my 1220 x 850 (with 2.2Kw spindle) router which was made by RNR Designs in Stockport.

If you Zip up the file and attach it I will take a look. Vectric posts are notorious for spitting out segmented arc's. I believe there may be a post-processor that is available which uses G2/3 arc moves so it might be worth taking a look at which post you used.

Thou to be honest any properly setup router should easily handle cutting what looks like a 10mm radius at 3mtr/min. Who set up the motor tuning, you or RNR.?
I don't know this company or the router but if it's built stiff enough and properly setup then it should easily handle cutting at those feeds.

[Robin Oakapple]

If you Zip up the file...

I'll do that tomorrow when I'm back in the workshop thanks