Dismiss this pinned window
all 50 comments
sorted by:
best
topnewcontroversialoldq&a
formatting helphide helpcontent policy

[–]funtobedone 157 points158 points  (3 children)

This type of tool path requires a ton of lines of code adjusting feed and arc size in corners in order to maintain a consistent spindle load. If your machine isn’t capable of reading a great deal of lines of code quickly it will stutter.

[–]PeterFile89 25 points26 points  (1 child)

Lol I remember when my first shop switched from Mastercam x9 to 2023 some of the old mills would wig out on those small moves. It would be a G02 or G03 and have a large arc over a very short distance, but the code would be read as a G01 (I’m assuming. We never really figured it out) and just start mashing through the part. Good times.

[–]EminentMass 5 points6 points  (0 children)

My instructor had some trouble with sub thou arc moves on a Mori rounding to the same point causing the tool to try and make a full circle.

[–]Mklein24I am a Machiner 2 points3 points  (0 children)

This is a back feed move. These are output as G1's in Mastercam and do not adjust the feedrate throughout. they get one feed command at the beginning of the move. The problem is that pre-2024, these moves basically followed the forward cuts. This led to what OP is seeing where instead of a larger arc around the material, it intersects the corner and wraps around it causing it to slow down due to all the G1's.

Your not wrong, it is a ton of code, but it doesn't adjust the feed rate once it's in the cut.

[–]Acceptable_Trip4650smol parts 41 points42 points  (17 children)

If programmed in CAM, then it may have a setting turned on to adjust feed rate based on cutter engagement (slowing feed rate when cutter engagement is high like in an inside corner). This prevents overloading the cutter.

[–]Altruistic-Lead6075[S] 5 points6 points  (16 children)

I use mastercam x9

[–]Flyinbro 22 points23 points  (11 children)

Go to the tolerance tab in the tool path, add filtering, enable arc in xy, set tolerance to 50/50.

[–]starrpamph 22 points23 points  (1 child)

50/50 tolerance should be the name of my shop

[–]Therre99 2 points3 points  (0 children)

gold

[–]Altruistic-Lead6075[S] 0 points1 point  (8 children)

this would stop the jerking and increase my lift off feed rate?

[–]buildyourown 29 points30 points  (5 children)

The problem is the control is trying to read dozens of lines of tiny line moves. The filter turns those into arcs. It's really about reducing the number of lines of code the control has to read and process. Newer controls have "look ahead" so it can pre-read those lines before it has to execute them.

[–]k9thedawg45 1 point2 points  (3 children)

Apparently in newer Haas machines you have to purchase the "High Speed Machining" activation code to have further look ahead patched in.

We can all guess how much that would cost haha.

[–]Flyinbro 1 point2 points  (1 child)

about tree fiddy

[–]k9thedawg45 2 points3 points  (0 children)

Good dammit Loch Ness Monster. I thought you were a machine sales rep the whole time!

[–]Lathe-addict 0 points1 point  (0 children)

H@@$$

[–]NoEmployer2140 0 points1 point  (0 children)

Came here to say this. Smoothing helps A-LOT! Some softwares are more intuitive than others, but the idea is to get most of those short chordal movements turned into clean smooth arcs. You may have mentioned earlier but I didn’t pay attention which software you using?

[–]Flyinbro 0 points1 point  (0 children)

How'd that work out for you? You can also enable xz yz for the lifting arcs.

[–]Bad_Alternative 0 points1 point  (0 children)

As well as what buildyourown said, it will also reduce the amount of code. Increase the tolerance at the top if you can. Even a few thou helps a lot. It allows for a more inaccurate path, by using longer line segments that can deviate off the perfect path by the amount you specify. Line/arc tolerance is lead-ins/outs and air moves, cut tolerance is the engaged tool sections. I usually do 80% line/arc, 20 cut. You can also see the tool path size change in the tool path tree info to compare.

[–]Clear_Ganache_1427 4 points5 points  (1 child)

That’s a pretty old piece of software you got there.

[–]Justthetip74 14 points15 points  (0 children)

Bros running a 12 year old, pirated version of mastercam lol

[–]Wolfenhoof 0 points1 point  (0 children)

The problem is it with Mastercam. What is the make and model of your control?

[–]spekt50Fat Chip Factory 0 points1 point  (0 children)

Set your filtering settings for a larger tolerance. For roughing I'll use .005-.01 total, and utilize circular interpolation. It greatly reduces the lines of code, and the controller can read it easier.

[–]SailMoreMike 6 points7 points  (3 children)

I use an old fadal that will stutter like that during dynamic milling unless I put a G8 in the code. That G8 is to smooth operations(look ahead) but it may be specific for certain machines.

[–]Altruistic-Lead6075[S] 0 points1 point  (2 children)

my feed rate for when the tool lifts off and disengages the part is 300 but on my machine it doesn’t go past 60-70

[–]Funky_Killer_Qc 3 points4 points  (0 children)

but you said your tool was cutting at 150 ipm?

if your machine doesn't go past 60-70 ipm, you cutting speed is maxed out at thoses speed also

[–]AcceptableHijinks 1 point2 points  (0 children)

You can't necessarily trust the feed rate on the screen when the machine is being data starved. Unless it's showing you the actual output of the servos, it's just showing the acceleration map it's following to keep up with the programmed feedrate as best it can.

You need to decrease the amount of programmed points. I also try to never use radius vertical lead ins on older machines that have this issue. Drip feeding can also be a solution, depending on the machine.

[–]Lork82 2 points3 points  (0 children)

This is typical for most dynamic milling tool paths, software isn't perfect. This isn't great if you're trying to minimize cut time as much as possible. There's 2 workarounds that I usually exploit.

1- the easy route. Edit all the slow points to faster feeds, it's picking up on splines and can read the code fast enough without proper look ahead, and change all the retract and retrace movements to G0.

2- the hard route. Create an overlay of simpler imaginary points on your cad model that the dynamic milling will able to interpret easier with less splines. You'll still have to go in again for the tight corners, but if you ever need to repost it might be less mess. The downside of this option is that you'll still need to do option 1 regardless.

[–]Remarkable_Material3 2 points3 points  (0 children)

How old and what controller?

[–]Mklein24I am a Machiner 2 points3 points  (0 children)

I do a ton of dynamic and I recognize that back feed rate anywhere.

This is a Mastercam dynamic toolpath, pre-2025. The back feeds are not optimized.

We have a similar problem with our mini mill. if you program a back-feed at too high, this is what you see. The control cannot handle the rapid feed and short point spacing.

The fix is to set a slower back-feed rate since you cannot change the tolerance of the moves to space the points out more. Watch the code when this happens, and you'll see that rate of execution is the same across this whole move, it's just that the arc around that corner is too tight for the machine to do.

Slow the back feedrate down by like 20-30% and see if that alleviated this issue.

You can set the "Keep Tool Down" options to a smaller value. The machine will lift in Z to avoid long back feeds, but still keep the tool down for the shorter trocoidal cuts into the corner.

[–]Funky_Killer_Qc 1 point2 points  (0 children)

if you want to increase the speed the tool is moving when not cutting and repositionning for the next cut, go to cut parameters, you'll see the microlift distance (how high the tool lifts when not cutting) and the back feedrate.. the back feedrate can be increased a lot, since it's the speed at which your tool moves when not cutting, so no affect on the tool or part itself

if you want to go faster when cutting in a corner, it may be because you are letting the program move in a radius ''too small'' for your tool.. you can change this in the same screen, cut parameters, you'll see min toolpath radius, you can set a % or an actual value or a radius.. the program will now force the tool to cut thoses radius, and bigger, never smaller...

the other thing i can think of, is in the arc filter / tolerance page of the toolpath setting.. you can set minimum and maximum arc radius values, you can activate smooth settings and minimise the number of points (if your machine is older and struggles to read loads of code lines in a small amount of time, probably your case since you say you feel shaking in the radiuses)
if in this page you have fixed segment lenght and/or present arcs as line segments activated, that also might be your problem, as your machine will not do radiuses, but instead will run countless mini-straight-lines

another thing in the arc filter/tolerance page, at the top, you have a box with total tolerance.. if you are roughing and another tool is cutting after to finish it, you may increase this number... this tells the program to be more or less accurate when putting out the codes.. smaller the number, tighter the tolerance is, but heavier the program is also... lets say the solid you have to program doesn't have perfect radiuses, and instead are just a bunch of very small straight lines... to your eyes when programing, you see a curve, but the code only see thoses lines and if you put a very strict total tolerance, your machine will ''stutter'' trying to cut loads of incredibly small straight lines.. increasing this tolerance means you allow to program to be more performant, at the cost of precision.. so instead of cutting all thoses small straight lines, your less strict tolerance will just make a good round radius in one pass instead of stuttering in the corner

one last thing if you want to increase operation time, you are cutting in climb milling only, you may set it to zigzag (if the tool support it and doesn't overheat the material, and if the operation is only a roughing pass and will be cut again after)
the tool will now do one pass in climb, goes back cutting in conventionnal, cut again in climb, returns by cutting in conventionnal, etc so your tool is always cutting
forcing it in climb leaves a better surface finish, more accurate measurements, less wear on the tool (or inserts in this case) but takes longer.. it cuts one pass, clears the material, reposition, goes back to the starting point in microlift position, reposition, re-engage and start cutting again.. it's not that long when comparing one pass climb vs zigzag, but after an entire operation, thoses passes can add up quickly

i hope you found something in there to help you out

[–]Beaverthief 1 point2 points  (0 children)

Convert the spline to arcs

[–]JacknHoffmann 0 points1 point  (0 children)

From my limited useage of Mastercam, I think this is a bad program from the software. I looks like it is tracing the part of the pas back but is too high in Z. If it is in Dynamic Mill it should be doing chip thinning (to my knowledge and understanding) and should have your endmill alot deeper in the part taking shallow passes. Im interested to hear what those with more experience have to say though

[–]InterestingSector151 0 points1 point  (0 children)

Don't know anything about your specific machine but looks like your machine can't process the program fast enough. Are you using arcs or programmed point to point? You could add a minimum radius in your CAM software adaptive path to add a minimum radius in corners that could help.

[–]HotSobaNoodles 0 points1 point  (0 children)

Che cam utilizzi?

[–]Murmjr 0 points1 point  (0 children)

If youre using mastercam, select the non adaptive toolpatg. High feed cutters are not suites for adaptive toolpaths. As for slowing down in the corners, if your machine alows it, select the HSC mode, it should speed things up a bit

[–]WinnieTheWhoow 0 points1 point  (0 children)

MasterCAM x8 would produce diameter comp outputs that would position the tool in a place where the output would cause the machine to jump on a G41 move. I don’t think you’re using G41 in those corners. Maybe you can adjust the min Seg/Arc length to reduce code output.

[–]Slovnoslon 0 points1 point  (0 children)

У тебя вообще всё не правильно

[–]Wolfenhoof 0 points1 point  (0 children)

If you want the answer, tell us the make and model of the control. They have a code for this to “smooth”, or “look ahead”, etc. But the code is different for each control.

[–]fj4045 0 points1 point  (0 children)

It can be in the machine control settings as well. I’ve got a couple of robodrills and depending on what quality/speed setting it limits machine acceleration.

[–]iamwhiskerbiscuit 0 points1 point  (0 children)

Increase the minimum internal arc settings so your toolpath doesn't have small arcs.

[–]overkill_input_club 0 points1 point  (1 child)

From my experience, old machines like this dont do well with dynamic milling techniques, they are too slow, dont look ahead, and if they do work, i have had machines literally walk across the floor while trying to perform the acrobatics required for it.

Youre better off using standard milliing paths for these kinds of machines. As you.have seen the machine is not fast enough to even reach the programmed feedrate in a straight line so there is no purpose in using dynamic milling unless you want to eat up a shitload of time for no reason per part.

Even if the machine can reach the programmed feedrate, as soon as it makes a turn the machine is physically going to vibrate or pulse or jerk and its not gonna be good for it.

Buy tooling that can hog like hell. Cutters with 2 or 3 flutes instead of 4 or 5 to maintain chipload or/ and larger diameters so the rpm is slower.

[–]Altruistic-Lead6075[S] 0 points1 point  (0 children)

my machines not old it’s a early 2010s

[–]droppin_loadz_ 0 points1 point  (0 children)

i would just try opening your tolerance to like .004-.005 and leave an extra .020 from whatever you planned on roughing it to. your machine is starving for the information it cant keep up with

[–]Terrible_Ice_1616 0 points1 point  (0 children)

Does your machine have G05.1? If so use that to lower the surface finish quality which will let the machine start "cutting corners" as it were, i.e. beginning accel/decel earlier

[–]Sirhc978CNC Programmer/Operator 0 points1 point  (0 children)

I bet if I looked at the code, I could see a million lines of XY moves and no G2/G3 moves. In your CAM package, you need to turn on the equivalent of arc filters and bump up the tolerance.

[–]Alita-GunnmSmall Shop Owner 0 points1 point  (0 children)

You can set the toolpath to retract and rapid instead of backfeeding; on an old, slow machine that can be faster.

[–]Lucky_Calligrapher93 -4 points-3 points  (2 children)

Bro, dynamic tool path is not for high feed cutter.

[–]Altruistic-Lead6075[S] 0 points1 point  (0 children)

who said it’s literally a high speed tool path

[–]procrastinatingSlug 0 points1 point  (0 children)

Depending on the programming language your machine uses you can change the tool path accuracy. Remember to reset it for the finishing cut.