Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: Raymondo on July 20, 2019, 08:17:00 PM
-
Hi
I am having trouble a Z feed does not get to zero before the next command starts to move and it seems to be feed dependant
G0 Z .25
G1 Z0 F55
X2.2 F100
this will start feeding the Z value until about .020" .030" before Z reaches zero then the X moves begins leaving a .150 to .200 long ramp
If I slow the Z feed down to say just 4 it seems to feed all the way down then do the X move
Do I have some thing set wrong some where
Regards Ray Hudson
-
This can be caused if you are running in Constant Velocity mode using G64. This causes the control to blend moves, and that is bad for drill cycles.
Try inserting an Exact Stop mode command, G61 before the drill cycle.
-
I use mastercam and I looked through and it is putting a G64 at the start of the code
Thanks I will test a G61 out tomorrow but am pretty sure you have the problem solved thank you very much
I think in the past in high feed moves I was getting larger radius on internal radius machining but could never figure it out so I think that will be the same problem
Regards Ray and thank again
-
I have tried the G61 and it cures one problem but it is so jerky doing compound curves etc that I can't use it
Also doing hi speed cut outs with G64 it cuts external 90 degree corners fine but internal corners 90 degree corners it puts a large radius instead of a sharp 90 degree corner and this radius is related to the speed of the feed so to my mind is not following the tools path and I think it is impractical to put a G61 before every internal corner and a g64 after and don't think the post processor could figure out to do that either
So I am at a bit of a loss how to tackle the problem
I am using a router and feed of 120 inch per minute and need to get down to say 6 IPM to make is follow the desired tool path
Regards Ray
-
It sounds like you acceleration is too slow. Try increasing it a little at a time. You may also want to look at the CV wizard.
Mike
-
I did not know about the CV wizard and will have a good play I have not found any real explanation of how it works and what angle 1 angle 2 etc should be set to and what is means but I will set up a test piece and test it out as best I can the docs that came will mach4 on CV do not seem to be what I have for CV wizard
Mine had angle 1 set to 179 and the rest to zero
Regards Ray
-
Run the CV distance tolerance wizard and read each screen............ the documentation is built in.
-
Hi
I open the wizard there is CV_feedrate there do not seem to be any help screens there but I can alter the angle0=179 to what ever I want
there is also the mctuningwizard this I can move the sliders up and down but can't save or in fact get out of it with out doing a Alt Cntr Del it seems to lock up I also cannot read the bottom text in the screen or scroll it up
This is on my home computer in demo mode I will try on the machine tomorrow
regards Ray
-
Don't overlook the possibility of dynamically switching between G61 and G64 as needed so that drills can be exact and regular moves get smoothed out.
-
Good point Steve and it may be exactly what he needs to do.
If you do not have mcCvDistToleranceV001 in your wizard list you probably need to update.
-
Thanks guys
I installed the updated latest program ran the CV Tolerance wizard
I had a pretty good machine before now it is transformed and truly great to use way faster much smoother
I tested it with some previous intricate cut outs I was doing and really was unaware these had minor problems it is so much better and so much easier and smoother and much faster
Thanks again WELL DONE
I have posted a few time and always been helped I believe Mach4 is a fantastic program but like all very complicated things that need to be configured to fit individual machines it is a leaning curve but having help available is a great thing and should neve be under estimated
Thanks again we are now all good
Regards Ray
-
:)
The CV distance tolerance wizard is one of the funnest things I have had a chance to do.
Glad it worked well for you.
-
looking at the numbers generated you would never do that by trial and error well not really good
I intend to have a further play with it my router is fairly high speed and I may have a go at tuning the motors for faster acceleration
I assume your wizard does calcs on accel and speed and a time and distance maybe
It is nice to have the machine working at its best the other option I have not tried yet is currently I have the tolerance set to .001" this could be increased for most work to say .005" I will test what difference that makes though at .001" the machine is really fast and exceeds the speed and feeds off the tools I am using
Thanks again Well done
-
Well, the CV table was given so that users could truly tune their CV behavior. For that it works really well and just as intended. But it would take a lot of testing and just plain work to optimize it. Some did it but most want something that will get them a lot closer a lot faster and easier.
It just uses accel of the included axis motors to determine the worst case. This is why when designing a machine, it's good to have as much accel as possible and that all axes can run at the same accel rate without issue. Without issue being the most important part. Knowing accel you can calculate bend radius at any speed. Knowing that radius you can then calculate the max distance from corner it would be at that speed for each angle. Naturally it does not take any machine design flaws (flex, backlash, etc.) into account so again, best to eliminate those in machine design.
Most machine to a tolerance. +/- .010 for example. They want to run the path as fast as possible while staying within tolerance. That was the whole idea of the wizard. Increasing the tolerance will decrease the run time and make it smoother but keep the path within the given tolerance. Unless something (like backlash or flex) lets it exceed the tolerance.
Thanks!