This week, my laptop that ran Mach 4 died. I got a replacement, transferred over the license and uploaded my profile.
First program I ran was a simple rotary axis program and had no issues.
Today, I had to run a program that surfaces a piece using scallop or spiral profile in fusion 360 CAM. Started running it but immediately it was only running at about 20% speed - the command was 250ipm but the actual was only 90 (as displayed in the current feed rate section). No matter what i set the feed rate over ride to (other than 0), it did not change the actual feed rate.
I did a bunch of stuff that didn’t work - rebooted the cnc and laptop, bought a new ethernet cable, uninstalled mach 4 and reinstalled it running the ethernet and performance program as well as doing all the configuration manually, verified the CNC code…. none of this worked.
The one thing I did that essentially covered up the issue was I applied smoothing to the program in fusion 360 in order to reduce the amount of programmed points. This worked great for the main portion of the program but towards the end, there was more detail in the piece which required more lines of code. When it got to this point, it went right back to what it was doing - slowed down from 250ipm to about 100ipm and the movement was shaky causing lots of machine vibrations.
I have lot of programs with very detailed machining and I have never encountered this problem until today. I usually never have to apply smoothing to the code either.
From all the diagnostics I have done, it seems as though the communication to the CNC is very slow so when the program is very code heavy, it cannot communicate fast enough.
I have a lot of CNC work to get through right now and cannot afford this so any help is appreciated!
Back at it this morning. Continue to have the same issues. Here is a screenshot from mach 4.
The program I am running this morning is even more detailed than the previous one. Even with smoothing applied, you can see the current feed rate is only about 10% of the command. And then once it hits a section where it doesn’t require the detail, it will bump up to the commanded feed rate
This is a weak point of Mach… Large and complex G code files can cause problems. This can happen because the computer/controller can’t keep up with the G code. It can also happen because of tiny segments of G code not allowing the motors to get enough time to accelerate. If it’s this problem you can tweak your acceleration settings to try and get some more performance out of it.
Hi Eric, I have uploaded a section of the G-code that is running the slowest - this is obviously a fraction of the 60,000 lines.
However, I don’t believe it is G-code related. On the previous computer, I had zero issues with running this complex code - it was in fact this exact program that I ran. The difference is the old computer I didn’t have to use smoothing in Fusion360, it handled it as is. The pasted program is with .001 smoothing tolerance.
The more I dig into today, the more I think it may be about the ethernet transmission speed. The new computer has a gigabit ethernet port but something is limiting the speed and I am not sure what.
My previous computer had a transmit buffer of 512 but was capable of going higher. The new computer is only showing a transmit buffer of 128 and I can’t seem to raise it. Similarly, the ethernet network settings are showing that the transmission speed is being reduced to 100Mb/s whereas it is capable of 1000Mb/s.
So it seems as though it may be a data transmission speed issue…. please tell me if I am wrong.
I am not running a smoothstepper - never had to on my old computer
More research is leading me to believe that windows 11 could be the issue - that’s what the new computer came with. Old one was windows 10. Reading a lot about gamers upgrading to windows 11 and having issues with slow communication
by Smoothstepper, Paul means the controller in the cnc control box, not anything on your computer. Since it’s Mach 4, odds are that you are running the Ethernet Smooth Stepper.
Ahh, thanks for educating me on that. I didn’t realize that I could change the configuration as I didn’t have to for my previous computer. I guess I have some more research to do
I’ve had this problem before. It was caused by Windows updating on my controller computer and it migrated the folder (in Documents) to the cloud. it took me a couple of days and a phone call to Avid for help to figure it out. The poor guy from Avid had to force me to read out the file path that I was opening my tool paths from because I “knew” that the folder was in my C drive. lol. I was as dumbfounded as the guy wasn’t surprised that my tool paths were being run from the cloud.
The Ethernet Smooth stepper is a 100 Base-T device, so even though your computer is capable of gigabit speeds, the best you can get is 100Mb/s speeds. (the lowest of the two). That being said, it should not be an issue if it is operating correctly. Even though you are only operating at 100Mb speeds, make sure you have a quality ethernet cable. I would get one rated for gigabit speeds, (Cat 6)
Also, make sure you ran the Avid CNC - SCU Application. It will setup your Network card for proper communication with the Ethernet Smooth stepper and optimize windows
I am considering it as I do want to upgrade the machine over the next year or two - add 4 feet to the length, upgrade to the new servo motor and auto tool change. Maybe the EX controller is the first step to start with - who is best to email in order to discuss the best way to attack this
Just use the contact form up top. That’ll make a ticket and someone will get right back to you. They can make you up a quote for exactly what you need. If you’re going from stepper to stepper the prices are very reasonable. One of the (many) strengths of this new controller is rock solid reliability.
For those interested - I have solved the issue. But I still have a question.
The solution to my problem was to calibrate the constant velocity setting in Mach4 using the constant velocity wizard. This has maintained my federates with a tolerance of 0.001” which is more than good enough for woodworking.
Question - for CV to be applied by mach 4, G64 needs to be called out at the top of the program. I don’t see anything in Fusion360. How do I go about adding this to the post processor?
