Mach 4 Acceleration/ Deceleration

I have Mach 4 running a 3d Finish toolpath with a lot of fine detail and the sudden stops and starts have the machine shaking all over. My assumption is I need to adjust the acceleration/ deceleration of the motors to make the movement smoother, but don’t know where to adjust. Can someone guide me?

Thanks,

-Eric

1 Like

The machine settings are the maximum the machine is capable of, not necessarily what should used in all cases. I wouldn’t mess with them unless you set them yourself. AvidCNC has pretty good starting numbers.

If you are seeing things you don’t like, adjust the tool path settings in the project. They are probably too aggressive for what you are doing.

In Mach4 click on the Configure pull down and select Control. Then select Motors on the next screen. Then click on the motor you want to change the acceleration on. That screen should show an acceleration selection window that probably is set to 50. Reset to 30-35 and click Apply and Ok.

2 Likes

can you adjust acceleration in aspire?

No, it is controlled by Mach4 and I know of no way it could be changed with a G-code command.

Acceleration isn’t your problem. Your speeds and feeds are though. And yes, they are controlled in Aspire.

Do you use a S&F calculator?

The default AVID accelleration settings (if they are still 50 i/s^2 or more) are fine for cabinet panels and other bigger stuff with not a lot of direction changes, but way too aggressive IMO for Vcarving, fine 3D carving, or laser work. I run at 15-30 for the less critical stuff, and on some types of laser work I go down to 10. It makes a huge difference on vibration and won’t affect your runtime much until you get down below 15. Your feed speeds will also affect vibration, but the impact you your job time there is pretty much a 1:1 relationship, so its good to start with accelleration settings first.

3 Likes

I second the need for acceleration changes to smooth out your machine in certain situations. I switch from cutting larger items such as panels to cutting inlays on guitars and jewelry boxes, etc. Inlay work definitely doesn’t like an acceleration of 50 with the constant directional changes.

So @jjneeb, do you have multiple installations of Mach 4 setup on your computer with different acceleration settings as defaults? Say one Mach4 install at an acceleration of 10 and one for 15-30? Or do you manually make the adjustments within the program each time? I use to do that when I utilized a different control (EdingCNC) but haven’t tried it with MACH 4.

Love your YouTube videos BTW. Good Stuff!

The ‘Avid CNC Mach4 Loader’ icon typically placed on your desktop will always load the Avid CNC profile. However, you can use the Mach4GUI.exe program located in C:\Mach4Hobby\ to make a copy of that profile and give it a new name (avoid using spaces). Now you can return to the desktop icon, make a copy of it and rename it similar to the new profile name. Now right-click on the new icon and edit the ‘Target’ field to replace the name at the end (default: AvidCNC) with the new profile name from earlier. You can open the new profile from the desktop and customize settings, never losing your original profile. Best of both worlds. Remember if you muck something up, that’s on you :smiley:

1 Like

Hi Paul,
Fortunuately the motor settings are not ones that require restarting Mach4 (unlike a lot of the ESS settings), so I just change the motor settings when I need to. I suppose if I did this a lot I would make another profile (or more likely I would make a button on my screen).
I have sorta setted on 15i/s^2 for my normal work. Then I’ll drop the Y axis to 5 or 10 when I’m doing some laser raster work (one of my lasers has a 0.002" spot and any vibration at all will show up in the work). One of these days I’m going to run an experiment that varies the accelleration times and measure accelleration and the Gcode execution time to get a more accurate impact. The other reason If you normally run really fast jog and feed rates you’ll notice the lower accelleration numbers sooner, but I usually feed under 100ipm and jog at around 50, so you don’t even notice the 15i/s^2 accelleration. You definitely notice 5 though :slight_smile:

That would make for a killer addition to your YouTube portforlio of videos.

2 Likes

I see people posting in many topics that they think “max acceleration” is the culprit to whatever problem they are having. It has become the boogieman!

Personally, I have never touched that parameter on any of the 6 CNC machines I own and I never see these issues. So this has peaked my interest.

I think it would be great if you all started posting video of the machine running as well as the g-code file it is running. Do include your setting for max acceleration.

Since you posted video and g-code, guess what? We can convince @Eric to have the factory start giving more insight on what everyone is dealing with!

So let’s get everyone who needs help on the topic to post a video HERE so we can all see. Just blindly throwing out “change yer max accel” without further insight doesn’t help folks.

NOTE: You can share videos and photos directly from your Apple and Google cloud accounts. Just use the “share by link” function in each of those services. You can also share using YouTube but that is much harder to do for folks that do not have an creator account.

1 Like

I dropped my acceleration from 50 down to 35 and that solved my issue. Why is AVID Support so adamant that that is not the issue? Solved it for me on this machine with Mach 4 and my older AVID machine running Mach 3. I agree with Jim that if I had a lot of long cuts, 50 would be ok, but I do a lot of small details with a lot of small vectors and slowing down for just one section of a job is not feasible,

1 Like

Take a look at this video starting at the 12:15 minute mark.

1 Like

Because it is a limit to keep your machine from tearing itself apart, not something you should see while cutting.

CAM software like Fusion 360 assumes a rigid machine and metal cutting thus calculates a low feed for lead in/out, ramps and helical operations. Then it will execute the rest of the cut at the feed specified for the tool. If you are using a wood or plastic cutting tool then that feed different is really large. You can also get this jump in feed rate while doing HSM for aluminum.

This difference in feed rates will cause a gantry machine to jerk around because the feeds are so wildly different (aka, your max acceleration is actually being used during a cut which is bad). On a gantry with low rigidity this tool pathing strategy makes for bad surface quality.

You need to keep the feed rate of your lead in and out, ramps, helicals all to within about 15% of the cut feed max. You will find the sweet spot for your machine by trail and error.

One reason why you would think your problem is solved with increased maximum acceleration is “rubbing.” Rubbing can give the appearance of a smoother surface to those who do not know what they are looking at.

What is happening is the CAM software calculated the feed based on chip load. When you override your machine’s ability to properly accelerate you will always have the beginning and end of your tool path cutting less than the optimal chip load.

You will experience rubbing as the distance traveled will be less than the ability of the cutter to make a chip. This will reduce the tool life, heat the tool and workpiece, burn wood, blah, blah. All that good stuff.

But new folks will think the surface quality is improved by the rubbing.

I have no idea what this guy is talking about. His machine is made of AvidCNC parts but it isn’t an AvidCNC machine.

He is using Teknic SD motors so any relation to what AvidCNC set as their configuration has exactly zero meaning.

I understand the slowing down changing the feed rate at the beginning and end and admit I never thought of it like that. It sounds more like a trade-off between the “rubbing” at the beginning and end of a toolpath vs. the shakiness of the machine.

I don’t believe I am driving my machine faster than I should. This is the 60x120 Pro with AVID Leg kit, Running an 1/8" end mill at 200ipm.

I did not experience this on my previous Pro4896 machine. That was supposed to be less rigid than this one.

Rubbing is ALWAYS bad so is never part of any tradeoff.

I too have a PRO60120. They are very large machines with very low rigidity. Essentially your in and out should be exactly the same as your tool feed. I drive around at the same “grandma” feed rate all over that gorgeous 5 foot by 10 foot workspace! Any change in speed just leaves a big squiggle every time its tried.

I thought the fundamental issue here was the effect of acceleration settings on machine stability/shaking. This video clearly shows that effect at several acceleration settings. His machine is an older machine purchased from the the Avid company prior to them adopting the name Avid. It is very similar but not identical to the present day PRO line. He changed out the NEMA 34 steppers to Clearpath servos. They allow a real time graphic display of motor acceleration in real time as is shown in the video, an even more objective measure of the issue than simply visually observing the shaking of the bed which is also shown.
I don’t know what more video evidence you want to investigate this issue. It might not support your narrative but is definitely relevant to the discussion.

Acceleration aside, there are a lot of tradeoffs between chip load that is ideal for the cutter lifetime, and surface finish. On a lot of bits (especially small diameter) the best chip loads (at least the ones advertised) will leave a pretty scalloped finish. I often run lower chip loads than recommended for a better finish (I don’t especially like sanding) on wood. Plastics are less forgiviing because when they heat up and melt it gets ugly fast.

The acceleration setting isn’t just to protect the machine, it is to manage oscillations in the chassis of the machine as well. You will always have some amount of time when the chip load is reduced when you change directions or start/stop. Reducing the accelleration just increases the duration of the reduced chip load. Its not a cure all for sure, the feed rate does also make a difference in the amount of vibration on direction changes, but if you only use feed rate, you can end up with some really long execution times because it will impact the long cuts and it linearly affects run times. When you have really eratic detailed stuff like Vcarving or laser work, you end up turning all the time and rarely get up to speed anyway. The accelleration can make a huge difference in vibration without a huge impact to runtime in these cases, especially with a laser.

So I think both feed rate and accelleration need to be managed to keep vibration at bay, especially on the really big gantry’s (mine is only 4 ft). I got a huge improvement in Vcarve quality dropping from 50 to 25, and when I started laser work I had to drop to 15 in acceleration on Y and X for use with my big laser, and then when I got the 50um laser, I had to drop to 5 when stepping the Y axis. It simply could not be fixed with feedrate (at least not one that would let me finish a simple picture raster in under a few hours).