[reg.miller]

Hi,

I was wondering how to better control feedrates on G2/G3 arcs when tool radius is more than half the arc radius.

For example. I have a 12mm slot with semi-cylindrical ends. I want to cut it with fairly large tool to optimise flexing and tool speed. However, the speed of the cutting edge will be advancing 3x faster than the tool axis cutting a 12mm diam arc with a 8mm tool . (The tool axis performs a 2mm radius arc.)

A 300% increase in tool cutting edge feed rate between the straight portion of the slot and the arcs.

How is this normally dealt with? Does better CAM software control feed rate of the cutting edge ?

Thanks for any knowledgeable person who can help.

[peteeng]

Hi Reg - Feed speed and cutting speed are related but it needs to be clarified to what you are trying to achieve? The feed speed & spindle speed are related by the chip load ie how big or small a chunk of metal is taken away each revolution by each tooth (chip load or feed per tooth) . The cutting speed is related to tool wear and the tool materials interaction with the material being cut. Some software can optimise cutting speed so it optimises tool life. Feed per tooth is important for surface finish and efficient cutting. Agreed in some geometry these do get messed up. Depending on your CAM system and your velocity planner settings will determine how the tool moves thru your slot end. What CAM and motion control do you use?

So cutting is aimed at :
1) roughing ie max material removal, hogging is one step up from that...
2) finishing ie best surface finish both require different tactics..
3) tool life again a different tactic..... Peter

[reg.miller]

Thanks Peter.

A change of 300% in cutting speed is obviously not good. It either means the straight sections are 3x too slow or arcs way too fast.

I got caught out by this when I set feedrate to 3mm/s on cut depth of 2mm. The first move is cutting with the full tool width of 8mm. That OK for roughing and about as fast as I want to go in view of the rigidity of the machine. When it did the arcs 3x faster, the machine was not stable enough. Maybe there's some rule of thumb about ratio of tool size to slot width.

I've seen other threads suggesting splitting the job but that adds quite a bit of extra work. Though that is probably what I need to do in my case.

I use FreeCAD and GRBL. FreeCAD is a good basic tool but does not have any means of adjusting for this kind of thing. I was wondering how this was dealt with in professional CNC machining. I may put in a feature request if there is an obvious way this is better dealt with in more advanced software.

[peteeng]

Hi Reg - The CAD does not plan the motion. Freecad will generate gcode, this is passed to a CAM system. Usually the code has a G64 in front. This is constant velocity mode. So the velocity planner then attempts to maintain constant velocity. The original gcode will have feed speeds in there like F1000 (1000mm/min) 3mm/sec is 180mm/min which is very slow for machining? 3D printer guys speak in mm/sec. So the velocity planner looks ahead and speeds up to the max set speed when possible. The planner will slow down at curvature changes like from a straight line to an arc. The path planner also moves the gcode points around a little but keeps them within the set tolerance of the planner. The grbl write up says it offers smooth acceleration and jerk free cornering. So I think you will find that changing some of your velocity and accel settings will cure your problem. V0.9 has improvements in arcs and in vel and accel settings so are you using the latest version?

Plus what spindle speed are you running at? and what material? 1F or 2F? at 180mm/min you are rubbing not cutting your chip load is so small it's wearing the material away. Learn about chip load, you will get much better results if this is correct for the tool and material...Peter

[deadlykitten]

hy reg 3x/300% may seem a large range, but if process is stable, then there is no issue

thus process stability and cutting specs range/variation are not corelated, thus there is no limit above which the process becomess unstable

thus cutting specs variation, subjective interpreted as big, may not be a major destabilization factor

---

peripheral vs core differnce is most relevant in application like a helix with a T mill, because tool is relative fragile in comparison to a normal end mill; if someone programed many normal mills, and suddenly encounters a T mill, then he may overload/break it, this is why this type of helix application is associated with recomandatioon for considering peripheral vs core

this aproach makes sense as long as side contact is < radius; the T helix example is meaningfull, but is not the only scenario for such a consideration

---

round slots, are under the category of toolpath with variable curvature, and most cams aproach begins with consideration of initial constant stock, to which it aplies of calculus or arch/peripheralengagement; for example, at corner, the contact length, among tool periphery, increases sudenly, only for a fraction

this can be treated differently, like reducing specs, or plunging the tool before starting the contouring operation

for a simple slot, the strategy can be g-code written, thus used a parametric aporach optimized for your machine

for more complex toolpaths, like hsm, etc, more things are to be taken into account / kindly

[the_gentlegiant]

Hi reg... I don't know what's going on here, but for some reason you're being drowned in a lot of excess knowledge, when all you're really after is how to adjust linear feedrates when cutting the inside of an arc. There is a simple formula for that. How to make your CAM apply it is something I can't help you with, but a calculator will do it.

For cutting the ID of and arc.

Internal Adjusted Feed = (Major Diameter-Cutter Diameter) / (Major Diameter) × Linear Feed


While we're here. This is the one for cutting the OD of an arc. (Where you need to speed up due to chip thinning.

External Adjusted Feed = (Major Diameter+Cutter Diameter) / (Major Diameter) × Linear Feed


I stole these formulas off the Harvey Tool website. Go there if you want to see visual references and related info.

[reg.miller]

Plus what spindle speed are you running at? and what material? 1F or 2F? at 180mm/min you are rubbing not cutting

So without knowing spindle speed or the number of flutes , you think you are qualified to tell me it is "rubbing".

Wrong.

180mm/min with full tool width and 2mm depth was throwing decent size chips outside the frame of the machine.

If you had taken the time to read the original post you would realise my problem is not "rubbing" but that cutting speed jumps by a factor of three in the arcs and is too much for the rigidity of this machine.

Try to understand the problem before jumping to conclusions and posting derogatory comments.

There is a simple formula for that.

Thanks GG. I already indicated that I know the ratio of the cutting speeds in relation to the diameters. That was the problem. My question is about how this problem is managed in pro machining.

[the_gentlegiant]

Thanks GG. I already indicated that I know the ratio of the cutting speeds in relation to the diameters. That was the problem. My question is about how this problem is managed in pro machining.

Hi Reg,

I guess I see in your first post how you were describing the adverse speed in corners problem, and by extension, your familiarity with the supplied equations.

So yes, if you're looking for CAM to do it for you, and your current CAM does not, then I think you've already answered your own question. :-) You need better, and likely more expensive software.

I program semi-manualy so bring those equations to play on a semi regular basis. I used to have this killer little app on my phone that made this as easy as could be, When I had to switch to a newer phone, the old app became incompatible. Only the icon remains to remind me of an old friend.

It would be simple enough to do a quick test in a trial CAM software. Have it helical mill out the center of a circle in an ever increasingly small radius. See if it pumps out feed rates that become slower and slower as it approaches the center of the circle. I've had quite a few jobs that needed just that, and with the help of the phone app, was always happy to hear the constancy of the sound in the the cut as it went round and round. OD ones are even funner, as things get faster and faster, and the coolant steam starts building.

BTW, I've been doing pro machining for many years. I think what you're after is hands off pro machining. I'm sure it's out there... if the price is right.

[peteeng]

Hi Reg - Sorry not meant to be derogatory. I'll be quite now. Peter

[reg.miller]

So yes, if you're looking for CAM to do it for you, and your current CAM does not, then I think you've already answered your own question. :-)

I'm aware my software is not handling this well. That is why I am trying to find out how this is usually handled in a more professional context. FreeCAD is FOSS, and this seems like something which could be improved. I'm looking to see how this is dealt with by those who've already solved the problem as a basis to see what to suggest could be done to handle this better.

Ensuring constant cutting speed seems relatively simple, at least in the case of circular arcs G2/G3. But there are probably some gotchas I am unaware of.

I think what you're after is hands off pro machining.

No. I could just open the gcode file and edit it by hand every time like it seems you do. It would be better if FreeCAD was modified to do this for me. That way I would not need to hand edit everything and neither would anyone else using FC.

[deadlykitten]

hy reg evolution is something like this :

... cam software :
...... raw code
...... feed mapping for :
......... each segment/arch/etc, depending on (at least one) : motion type, geometry type, mrr, etc
......... in-between segments/arches/etc : generally, load peacks are at joints, not among the element; thus the transition has to be handled
......... in/out movements : when tool enters/leaves material, there is a shock associated which is > normal in cutting

... cnc machine :
...... functions based on load monitoring, able to modulate feeding ( more than once for a single block ) : stop, decresese, increase

... advanced stuff :
...... software with cnc motion algorithms ( can generate g-code in respect to machine capability,avoiding 2 low or 2 high specs )
...... expensive cnc functions
...... applications that modulate a program in respect to cnc trial runs

---

for a simple pocket, one could write a parametric aproach, and make it specific to his needs

but some aspects can not be handled easy by a macro, like, for example, the real mrr can vary a lot ( starting high and ending low ), thus there may be considerable variations only when executing a single block

simple aproaches only modulate based on some generalitsic settings, empiric formulas more advanced ones take into consideration more variables

you can simply imagine the things you would like to improve write them down, and arrange those :
... i can do them fast
... i can do them in a bit more time
... i can't do them now, but i know is possible, at least should be ?!
... this idea is ok, but too expensive
... this is a wild idea, i wonder if there is something out there

the way you put it now, you will receive generalitics replies once you will go for an exact method, things became specific

---

in respect to pockets, this are the things i checked recently :
... g-code macro
... pc generated code ( y lathe )
... functions for compensation on tool center, tool side, with g41/42 or system variable, for a multitasking machince

feel free to ask anything / kindly

[reg.miller]

feel free to ask anything / kindly

There is no shock transitioning from a straight to a tangential arc. The principal question I'm trying to find out about is how this massive increase in cutting speed over feedrate is handled.

If tool diameter is > arc radius the cutting rate will more than double. That is likely to go beyond whatever range of values is acceptable for a particular job.

One option is to split the job and maybe cut the arc sections first. That is a lot more effort so I'd guess there's a better solution probably integrated into more advanced software.

Maybe I'm not getting much sense on this because machinists either do hand modifications, or it's all automatic and they are not even aware of what the software is doing for them beyond that it works great and produces the right cutting and feed speeds.

[the_gentlegiant]

There is no shock transitioning from a straight to a tangential arc. The principal question I'm trying to find out about is how this massive increase in cutting speed over feedrate is handled.

By lowering the feedrate at or nearly so to the start of the arc. For one thing I don't think it's normally referred to as cutting speed but engagement angle. How far around the tool does the radii wrap itself?

Fanuc has a function called Automatic Corner Over-ride that does this automatically. Because I never use it, I can't recall the G code for it. There are parameter settings for activation distance before and after the control notices a tight spot approaching. Settings for the feed to be adjusted by a percent, angle min/max to be considered for action, and also some time constants for adjusting Acceleration Deceleration profiles.

When approaching a radiused inside corner, there is a practical limit as to how big of a cutter should be used com-pared to what can be used. I try to go at least 1 1/2 to 2 times smaller diameter that is normally available in cutting tools.

Tight corners are tough for everyone. They can be rough drilled out. It may take 3 ever shrinking cutters to create simple a pocket with small radii corners. I get the feeling you're looking for one and done. It seldom works that way, even with HEM profiles where you attack it full depth with smaller cutters taking baby size radial bites. Tight corners are a *****, and I wish they'd drill that into Engineering students heads.

[deadlykitten]

There is no shock transitioning from a straight to a tangential arc.

not always, maybe there was none in a recent cut of yours, but can happen, even for a slot

in general, a tangential joint is not a guarantee for zero shock; also, a 90 degree curve, is a not a quaratee for a big shock; depends

how this massive increase in cutting speed over feedrate is handled

i have less wories for such, as i simply program them how i wish; you can struggle finding the inner workings of a software, or simply try another cam more frienldly to your style, or another aproach

Maybe I'm not getting much sense on this because machinists either do hand modifications, or it's all automatic and they are not even aware of what the software is doing for them beyond that it works great and produces the right cutting and feed speeds.

the moment you begin question methods, is a good start what you are discussing, is strategy aproaches; you may take a slot and an endmill, and try different methods, and/or ask for aproach methods from other guys, so to have a larger perspective on same operation

Tight corners are tough for everyone. They can be rough drilled out. It may take 3 ever shrinking cutters to create simple a pocket with small radii corners. I get the feeling you're looking for one and done. It seldom works that way, even with HEM profiles where you attack it full depth with smaller cutters taking baby size radial bites. Tight corners are a *****, and I wish they'd drill that into Engineering students heads

indeed, you can drill the corners before, and should work as long as the drill won't wobble too much; for example, if you wish to leave a stock of 0.1mm, and the drill will deviate/go sideways, then this may leave a mark on the final part, etc ... drill wobbling is an issue, as for same diameter and length, an endmill is much more rigid then a drill, so ... hmm

on some operations, i like to plunge the endmill before contoruing, but simple as it sounds, actually the plunge position may shift with radius wear offset, so is triky to take into account such things

i can take a code, filter the small arches out of it, change strategy only for them, or overall .... do something to make it perform more smooth at the machine / kindly

[reg.miller]

For one thing I don't think it's normally referred to as cutting speed but engagement angle.

engagement angle is important but it is not another name for cutting speed. On the first cut in a slot the engagement angle is 180 even on the straight section. That is not what is determining the change in tool cutting speed.

Fanuc has a function called Automatic Corner Over-ride

Thanks. That's the kind of info I'm looking for. So in that case it's done in the controller via a manufacturer specific Gcode. ( G41/42).

All accel/decel parameters apply to any speed change and are part of the planner, even in simple controllers like GRBL. That's not G41 specific.
Having a specific Gcode makes sense applying this punctually where needed. I would guess there are other solutions where it is done in the CAM software.

I try to go at least 1 1/2 to 2 times smaller diameter

Sure but that has a price. If I'm doing a deep hole, I need long, stiff cutter no a thin one just so that I do not have to worry about speed changes.

[reg.miller]

not always, maybe there was none in a recent cut of yours, but can happen, even for a slot

What I'm saying is that there is no shock because of a tangential arc. There may be a shock coincident with a tangential arc for another reason.

as i simply program them how i wish;

So your solution is to hand code the change , not rely on either CAM or controller features. Maybe that is often less trouble, or the only options. Thanks.

if you wish to leave a stock of 0.1mm,

I would not go within 0.1mm of anything with a drill ! He was talking about roughing out and thus avoiding the inner cuts of the arc where the cutting speed can get multiplied up by several times.

[deadlykitten]

So your solution is to hand code the change , not rely on either CAM or controller features

i can automatize and generate the code; as for simple slots, a cam is too complex

for example, i may have my own aproach on cutting a slot but if someone asks for something else, or has a different vision, i simply code it

in the end, you and up with a set of predefined methods for a single type of operation

code layout may be simple, linear, or look like a hand written macro; particularization on demand

Fanuc has a function called Automatic Corner Over-ride

if there is no such cnc function available, i can modify an existing code, to make it decelerate before a corner; decelaration may be simple, or curvature related, etc; process is automatically, using an algorithm, so a big toolpath size can be edited quickly

in case it matter, this had been done looong time ago, by different persons; is not new

---

as a side note, now i have to deal with a part, that has some tolerances and condition that do not go well togheter, would make the parts not possible to be assembled, even if conditions are respected

one part, out of 20, simply has too much deviation ( it popped up yesterday ), even if still ok, in drawing condition; to avoid guessing at the machine, i can calculate how much modification is needed, and where to aplly it / kindly

[reg.miller]

Yes, for simple forms, I find I often hand code rather than waste time configuring CAD. I get cleaner faster code with less unnecessary retractions.

[reg.miller]

this had been done looong time ago, by different persons; is not new

I was sure it was done a looong time ago by loooooots of people. That is why I was asking what methods were used. That was the start of this discussion.

I have now modified FreeCAD to proportionaltely reduce axis feed rates. Now for some testing.

[servtech]

Hi,

I was wondering how to better control feedrates on G2/G3 arcs when tool radius is more than half the arc radius.

For example. I have a 12mm slot with semi-cylindrical ends. I want to cut it with fairly large tool to optimise flexing and tool speed. However, the speed of the cutting edge will be advancing 3x faster than the tool axis cutting a 12mm diam arc with a 8mm tool . (The tool axis performs a 2mm radius arc.)

A 300% increase in tool cutting edge feed rate between the straight portion of the slot and the arcs.

How is this normally dealt with? Does better CAM software control feed rate of the cutting edge ?

Thanks for any knowledgeable person who can help.

In the good old days we could simply use G09 or similar if available.