Mach3 Feed Rate Help...

[Smash]

Dear All,

I have recently converted a milling machine to CNC. Everything seems to run great but I just can't seem to get the feed rate to match the settings I set in my CAM software.

I am using DeskProto for my CAM software and Mach3 to drive the mill. If I select a feed rate of 2mm/sec in the CAM software then run the Mach3, the feed rate is incredibly slow, approximately 1mm travel in about 17 seconds?

I assumed this was an issue within my CAM software post processor setup but I got the following response from their forums suggesting it may be a setting in Mach3? I am totally lost!!!

DeskProto response below:
"DeskProto handles the feedrate in a very simplistic way: it just copies the number that you enter to the NC file, without checking any units. So when you enter 2 in the Operation parameters for the feedrate, DesProto will write "F2.0" to the NC file.

The units are only for the user interface, DeskProto does not make any conversions here.
So the question is which units your machine needs for the feedrate, you then can make DeskProto show the correct units.

The numbers that you mention do nor yet tell me which units are needed:
1 mm in 17 seconds is about 0.6 mm/sec, or 3.5 mm/min. I cannot convert that to 2 in any other units. I hope you can find this in the documentation of the control software that you are using."

If anyone can give me some pointers I'd be extremely grateful!

I know there are a lot of experts on here that will solve this in an instant.

Thanks guys...

Best Regards,

Smash

 

[DICKEYBIRD]

I'm no expert but it sounds like you have something wrong in Mach's config. Maybe it's set up in inches instead of mm? Is the motor tuning correct, ie: a manual 25 mm axis move command gets you a measured 25 mm movement?

Only other thing I can think of is you have the Feed Rate Over-Ride set way low? It should be

("Smash" Great name for a CNC noob! I should change mine to "Expert Smasher!")

ps: See if your code has a G95 at the start somewhere. That'd put it in the feed per rev mode. Bet'cha that's it!

 

[Scott_M]

Hi Smash

I think the best way to go about this would be first check the machine and not include the CAM in the test.

If you type code into the MDI and measure and time it , it will tell you if it is the machine settings.
Pick something slow so it is easy to measure.

Set a scale on your table and put a pointer in the spindle and line it up with your scale.
Type G21 into the MDI line and hit enter. Just to make sure it is in metric mode.
Then type G1 X 25.0 F25.0 and hit enter.
It should take 1 minute to travel 25mm.

Let us know what it does.

Scott

 

[RonGinger]

Have you tried reading the mach installation and config manual? It has an excellent, step by step procedure for setting up correctly.

Sounds like you intend to be in mm mode- did you set mach to mm mode? That is the very first setting that must be made, all else depends on it.

Have you tested your leadscrew calibration? Use an accurate indicator or set of gauge blocks and measure a move, using cammands input on the MDI line.

Forget CAM software until you have verified all the basic machine moves.

Another suggestion is to take mach questions to a forum that is only mach- either the machsupport.com or the yahoo list. That is where all the real mach experts hangout.

 

[Smash]

All,

Many thanks for all of your help and suggestions, I am really grateful.
So far as set up goes, I read through the Mach3 manual and viewed a number of video tuitions before attempting to set the machine up as I didn't want the embarrassment of wrecking the machine.

Native units were set to metric and everything calibrated great and I am really happy with its accuracy. The motor tuning for X and Y axis is 2000 steps per mm with maximum velocity of 600mm per min.

The problem for me is that I am completely new to CNC, although I have read a couple of books on the subject, I am far from being an expert.

DickeyBird (great Name)
I have checked the feed rate override and it is runs at 100%
I also checked if there was a G95 statement within the code but couldn't find one, shame as this sounded a potential easy fix.

Scott, good idea to abandon the CAM and code direct.
I entered the code you suggested and all worked perfectly 25mm travel in 1 minute. So I guess this suggests it is something to do with the CAM side of things?

RonGinger, thanks also for your suggestions. I did try and register for the Mach forum but there may have been an issue with their site as part of the registration is to orientate 3 images the right way up using some sliders, I couldn't get the sliders to respond after several attempts so gave up.

I really appreciate all the help and feedback. Any suggestions on where I go from here?

Thanks again guys...

Best Regards,

Paul

 

[DICKEYBIRD]

I have checked the feed rate override and it is runs at 100%
I also checked if there was a G95 statement within the code but couldn't find one, shame as this sounded a potential easy fix.

Oops, now that I think about it G95 would've made the effective feed rate way too fast instead of slow. F2.0 after a G95 would've given 2mm per rev....pretty fast!

I think the search function on the Mach Support forum works without being logged in so you might rattle around there & find your answer. I always learn something when searching through old posts. Just about everything that can go wrong has been covered at one time or the other. Keep trying to join up though because you're gonna need help at some point from the guys there. What a stellar bunch they are!;D

 

[Scott_M]

Hi Smash

Could you possibly post the code that was giving odd behavior ? Maybe we could spot what is throwing things off.

Scott

 

[idahoan]

Hi Smash

Is the decimal point missing from the feed rate in the posted code (F2.XX); I have had similar problems if the point is missing, it will feed at a crawl.

Dave

 

[RonGinger]

I checked with Scott, the guy that runs the machsupport forum. There is a known problem with Internet Explorer 11 that does not work with the sliders. All other browsers and earlier version of IE work OK. Good old Microsoft, 'fixing' their latest browsers to fail with the rest of the worlds software.

 

[Smash]

Guys, many thanks again for all your help and assistance.

I thought about the problem today and convinced myself the issue must be with the CAM software seem as the code typed directly into the MDI worked fine. I changed the postprocessor setting for federate from mm/sec to mm/min (perhaps something I should have tried earlier).

Anyway, I am so happy to say that making the change has now given me the desired federate (simulated off line). I can't believe I have been so dumb and can only apologise.

Ron, I have now registered on Mach support using an older version of explorer, thanks for checking that out and letting me know the problem.

I have also ordered a new book on CNC programming and g-code.

Thanks also to Scott for the offer to review the code and to Idahoan and DickeyBird for their input and assistance.

I can now finish my little engine!

Cheers guys and many thanks!!!

Best Regards,

Smash...

 

[DICKEYBIRD]

Thanks for posting the solution Smash. Many people forget to do that.