Arc slowdown - a typical BobCAM head-banger

A job so simple I prepared no extra blanks, only the exact number of waterjet-cut blanks as what could possibly go wrong. Just a bunch of 3/8"-16 form-tapped holes in steel - spot, drill, chamfer mill, tap. Both the spot and chamfer ops done using a carbide 1/4" 90 deg spot drill.

On the final part, the carbide spot drill broke, and so the drill made an off-center hole, and the tap broke in the hole. But why on earth would the spot drill break?

It broke because I forgot to set "arc slowdown" for the chamfer mill op. For that op, I like to plunge close to the hole center, with a 170 deg arc tangential lead-in. The arc traversed by the center of the cutter is very small - and so the effective feed rate where the cutting happens is some multiple of the programmed feed rate. For a reasonable chip load, the feed needs to be ~20% of the feed rate for a straight-line cut. So here I figure it was taking a .010" per tooth cut, thin ice, worked for ~40 holes but in the end was too much for a 1/4" cutter.

BobCAM even in its latest greatest version still provides no assistance for simple feed adjustments - you're expected to do the math manually based on the difference btw. the part edge radius and the programmed toolpath radius, and depending on the circumstances, either enter an arc slowdown %, or just enter a proportionately slower feed rate.

This is basic, the only problem is it was such a simple part, I forgot to do it.

Anyway, so how do the other basic / low end CAM packages address this? How far up the food chain do you have to buy before the CAM automatically calculates reasonable feed rates for arcs, in particular, with awareness of which side of the part line the cut is on? One of the reasons I think BobCAM does not do this is because it's generally stupid about which side of the part line the cut is on, i.e. not able to distinguish whether it's an increased feed rate because it's a convex feature, or a decreased feed for concave.

Having used no other CAM, hard to tell if I'm an idiot for using BobCAM or an idiot for forgetting to take into account such a basic detail. Or perhaps an idiot for not realizing BobCAM can do it but I just don't know how. Hard to imagine folks putting up with this much fuss and inefficiency in complex parts.

How much time are you really saving by posting 2 different feedrated for a chamfering op? You want to feed fast on the lead in and then reduce for the arc motion...on a lot size of 50pcs? Sometimes slower is faster and this is one of those times.
I would not blame the software.

I use Surfcam Traditional and afaik, there isn't an option to do that.

However, I do have my posts setup to do this. I have it set to adjust feedrates on arcs, only if cutter comp is enabled. Generally I only use comp for finishing toolpaths - I don't want or need it to adjust feedrate on everything. Many times it isn't needed, and on toolpaths like adaptive stuff, that is already taken into account.

I like it because the programmed chipload is always the actual chipload when making finish cuts. Helps when making small arc moves in corners, or even making profile cuts on the outside it will speed up some depending on arc to cutter dia ratio. I have noticed it has helped make slots closer. Sometimes when using a large tool and making small arc moves at the ends, you can end up with a slot which is under-size on the length, but width is to size.

I think most machine controls can do this automatically, but might require the actual tool dia setup, where I program to tool centerline and only use wear adjustments at the control.


On chamfer tools with a sharp point like in your example, I don't use this (I mostly use them for deburring and there's usually no point to adjust feed on deburring ops.) If chamfering a hole for a tap like you, I'll just figure the feed manually and just program it slower.

Most of my experience is with Gibbs, OneCNC, and Mastercam. None of them had arc feed rate adjustments as standard, it was something you had to modify in the post. Sadly, I have found that over 98% of machinists don't even understand the need for it, which is likely why it is not widespread in CAM systems.

Mastercam recently came out with this option in a couple of toolpaths, but it is missing from most of them, and certainly the ones where it is likely most useful like circle milling and thread milling.

I finally got sick of always hand calculating this so I am paying to have my post modified to do this in Mastercam for all of the 2d toolpaths, including highspeed.

I'd suggest don't cut the chamfer with the tip of the cutter, use the beefier part of the cutting edge that can take a higher chip load and has the gullet to form the chip in. A spot drill is not what I'd use to mill the chamfer with anyways, not enough clearance relief IMO, but I don't know that for fact. A spot drill only has two flutes and has almost no gullet at the center.

Why not just spot drill deeper with a larger spot drill and eliminate the need for an extra operation

Arc slowdown is not for the way you are trying to use it

If you are challenged by correct speeds and feeds pick up a copy of HSM Wizard

"BobCAM even in its latest greatest version still provides no assistance for simple feed adjustments"

I don't know about that,you can manually edit all parameters

"It broke because I forgot to set "arc slowdown" for the chamfer mill op."

NOO,,,,see Who Flung Dung above,,,spot on spot

I am pissed because I can't take a photo and have BobCad automatically do the CAM

Blame BobCad,,,that's silly

"because it's generally stupid about which side of the part line the cut is on"


The center of the green line represents center of tool
I did same tool path 3x
no comp,left comp,right comp
does that help


" Hard to imagine folks putting up with this much fuss"

Yes it is,quit doing it to your self

" But why on earth would the spot drill break?"

Geez,that is what the whole question should of been about,not BobCad did not read my mind
Bad machinist practices come to mind
you "FORGOT" to set a percent of slowdown and///or you did not edit your parameters
But,,,SEE WHO FLUNG DUNGS post above,,,BINGO
Willing to bet the cutter loaded up and also rubbed (no clearance) so was trying to burnish your chamfer (lots of side forces)

Dave Cross said:

Most of my experience is with Gibbs, OneCNC, and Mastercam. None of them had arc feed rate adjustments as standard, it was something you had to modify in the post. Sadly, I have found that over 98% of machinists don't even understand the need for it, which is likely why it is not widespread in CAM systems.

Mastercam recently came out with this option in a couple of toolpaths, but it is missing from most of them, and certainly the ones where it is likely most useful like circle milling and thread milling.

I finally got sick of always hand calculating this so I am paying to have my post modified to do this in Mastercam for all of the 2d toolpaths, including highspeed.

Click to expand...

Bob has it and has had it for a long time,however a human must also push a button to make it come into play,,which is the way at least I wanna use it

Going off on a slight tangent, Dave Cross's comment about machinists not understanding the need for arc feed adjustment started me wondering.

Isn't this basically handled by the look-ahead functionality in modern controls? I would think machines designed for HSM work or mold surfacing etc are especially dependent on the control constantly adjusting programmed feed rate for improved surface finish. So would a machinists used to these modern machines ever even need/learn about this functionality?

Or maybe I misunderstand what is meant by arc feed override?

In Topsolid you can choose to maintain a constant feedrate/decrease feedrate in angles by a couple of different methods, but you do still have to *choose* to do so. I suppose that you could save this selection as a default behavior....now that I think of it. I still use this on occasion even with controls that have lookahead enabled.

Cheers, B

This is a chamfer for a 3/8-16 thread he is talking about

carbonbl said:

Going off on a slight tangent, Dave Cross's comment about machinists not understanding the need for arc feed adjustment started me wondering.

Isn't this basically handled by the look-ahead functionality in modern controls? I would think machines designed for HSM work or mold surfacing etc are especially dependent on the control constantly adjusting programmed feed rate for improved surface finish. So would a machinists used to these modern machines ever even need/learn about this functionality?

Or maybe I misunderstand what is meant by arc feed override?

Click to expand...

The arc feed slow down is ideal for doing slots or pockets.The tool will go full feed in the straight aways and slight arcs or splines,,but when it comes to an inside corner,so to speak,you can assign a percentage to the tool to slow down for it.Default is %100.If you want to use it you actually have to enter the percentage you want for it to work.OP is wondering why Bob does not automatically do it,because that is his reasoning he scrapped a part because he forgot to.

Dave Cross said:

Most of my experience is with Gibbs, OneCNC, and Mastercam. None of them had arc feed rate adjustments as standard, it was something you had to modify in the post.

Click to expand...

Gibbs has had it for years. Plug ins>HSM> Change speeds and feeds. Yes you need to do it for every op you care about but not every op requires it.

carbonbl said:

Going off on a slight tangent, Dave Cross's comment about machinists not understanding the need for arc feed adjustment started me wondering.

Isn't this basically handled by the look-ahead functionality in modern controls? I would think machines designed for HSM work or mold surfacing etc are especially dependent on the control constantly adjusting programmed feed rate for improved surface finish. So would a machinists used to these modern machines ever even need/learn about this functionality?

Or maybe I misunderstand what is meant by arc feed override?

Click to expand...

Most controls allow for some sort of "arc feed adjustment", though it is not often used, it is certainly more convenient to turn on and off in your cam system than it is on the control. HSM look ahead and slow down options are based on the maximum velocity a combination of axis can maintain a deviation from a user defined tolerance. While both methods reduce the feedrate on an internal corner, they are doing it for different reason and they will both have different values.

jrmach said:

Bob has it and has had it for a long time,however a human must also push a button to make it come into play,,which is the way at least I wanna use it

Click to expand...

I agree, this should be something you turn on or off for each tool path depending on your needs.

Hazzert said:

Gibbs has had it for years. Plug ins>HSM> Change speeds and feeds. Yes you need to do it for every op you care about but not every op requires it.

View attachment 238418

Click to expand...

I hadn't seen that before. It has been about a decade since I have used Gibbs, I'm not sure if that was there then or not. Does it work for all contour shapes, or only sharp corners?

@David, all shapes external or internal as far as I know and can do both sharp and tangential tool paths.

Good to know, thanks Hazzert.

I might be dense, but a slowdown in a corner has nothing to do with what the OP is asking about.
He wants a slowdown in an arc, just because it is an arc, while the corner modifications as shown on the Gibbs post are for slowing down on internal corners and speeding up on externals
due to higher/lower chiploads.

Seymour, the tangential option will slow down the feedrate on any curve ie, ports or other variable geometry. I have never tried it on a circle.

Sharp corners however you are correct, it’s for the high angle of engagement.

It appears the OP vanished,,but his thinking was off with his plan of the grand scheme of things

Jesus my Anilam controlled mill automatically adjusts feeds for arcs and it runs on win3.1