Speeding up the process

[flankbell]

Just a quick question to check my thoughts.

I need to cut a 1.5 inch deep pocket 7x12 inches with a 3/4 inch bowl bit for a customer. I do this all the time and have gotten speed and pass depths where it won't stall the machine. I had a thought though because it takes a long while with multiple passes, if I increased the step over from 10% to say 40% for the first 1 7/16s, and then created a separate toolpath for the last 1/16 with a 10% step over to clean up the pocket. Does anyone see a problem with this that I don't?

Thanks,
Tim

[tomgardiner]

This would be a better strategy, however if your machine is stalling then a larger step over will add to your troubles. You may want to try the clearance pass with a 1/2" straight bit at a higher feed rate leaving a generous allowance around the profile and for depth to make sure the square bottom doesn't cut into the corner radius. You can check different feeds and depths of cut without cutting by hovering over the toolpath list and seeing what the estimated machine time would be.

[martin54]

If you do a search on the forum you will see that I have mentioned this a few times, just be aware that if you increase the stepover then you may need to adjust your speed feed & depth of cut settings if you are close to the limit of what the machine can handle but if you are not having to alter your settings on the fly for your first pass then there shouldn't be a problem. Once you have your 2 toolpaths then merge them & output as one toolpath

Just had a thought that this process might not be completely the same using a bowl bit, sure I remember seeing a post from adze_cnc about it a while ago so before you go ahead with what I have said you might want to do a search on the forum or wait until he makes a comment on this post

[adze_cnc]

Would the speed need to ba altered at all? For the first run of a pocket toolpath the bit is engaged fully in the cut. If it’s not stalling or otherwise affecting the machine then a 10% or 40% shouldn’t matter. It might run harder on 40% though.

If you trust the flatness of your bit do you need a 10% stepover for a better surface finish?

One thing to note is that if you do a last separate pass be careful how you set it up. You need to set a start depth of 0 inches, a cut depth of 1.5 inches, and alter the pass depth of your bit to be 1.5 inches.

If you set a start depth at 1-7/16” and a cut depth of 1/16” you will end up with a pocket larger than what you want. With these settings the software thinks your pocket’s wall is only 1/16” high and moves the bit outward to have the rounded portion come into contact with the top of that wall. In general if the cut depth is less than the radius of the rounded portion of the bit you need to be aware of this.

Not having a bowl bit I would accomplish this with three toolpaths:

1. pocket using the original rectangle cutting to the top of the desired round (end mill)
2. pocket using a rectangle offset inwards by twice the radius of the round portion of the bit going from the previous depth to the full depth (end mill)
3. profile using the original rectangle (ball end). This case can use start depth of full depth less the bit radius and cut depth of the bit radius.

And now for the mutual admiration portion of our programme… martin54! martin54! Rah, rah, rah! Yay!

[Leo]

I would like to know more about the machine - spindle HP - workholding - DOC
What material are you cutting - steel, aluminum, wood, brass

Do you have an 11 HP spindle on your FMT Patroit machine. Is so then a 10% stepover is miniscule.

From what I see online your machine is a workhorse - why is it stalling out.

That pocket should be a couple of minutes in wood.

Do tell a bit more about your issue, machine.

EDIT IN
OOPS - sorry - my bad
I was looking at the wrong post - you do not have a FMT Patroit machine
Axiom i2r

[martin54]

Would the speed need to ba altered at all? For the first run of a pocket toolpath the bit is engaged fully in the cut. If it’s not stalling or otherwise affecting the machine then a 10% or 40% shouldn’t matter. It might run harder on 40% though.

If you trust the flatness of your bit do you need a 10% stepover for a better surface finish?

That's why I asked if the speed & feed were being altered on the fly, I sometimes slow down my machine for the first full engagement pass using the control software settings
If they are not then like you say there is probably no reason to alter the settings at all

I knew I had read something you posted about using 2 toolpaths with a bowl bit I don't own any bowl bits & generally do this with a normal endmill. I use bottom-cutting endmills & you would think the stepover wouldn't make a difference if the machine is set up correctly but I have noticed I get a better finish with a smaller stepover, never as low as 10% but generally somewhere between 15 -25%