[kvom]

are yous guys using radius comp for feerate with Mach3. Without it the 4th will only run at teh commanded feedrate.With it on it COMPS the A feedrate based on the diameter to better blend the A speeds to the linear axis(XYZ). It will use teh full motor tuning of the A axis to do this BUT it will be limited to the max speed of the A axis. For the best results with 3d milling on the 4th a ratio of about 6:1 seems to run best. Any more seems to be limited on speed and less you loose holding power on the 4th.

Without 4th axis radius comp it reminds one of watching paint dry, painfully slow(;-).

Just a thought, (;-) TP

Just did some tests in the shop. Setting the Radius in the Settings tab did absolutely to affect the time of a coordinates A/X move. I did increase the motor speed to 1500 from 200, which greatly increased the rapids, A 45 degree 1" line on a 3" diameter workpiece took 8.5 minutes at F15, a move that takes 4 seconds on a flat plane. It seems to me that Mach3's trajectory planner is not working properly here. If I change that move from G1 to G93 G1 F15, then the move does take 4 seconds. However for engraving, all the moves are very short, so to use G93 each G1 would need a different F word based on the move's length. The CAM wrapper I use doesn't support this conversion.

Unless I can find a Mach3 setting to coordinate the axes better I am at a standstill.

[VTX1800]

Hey guys,
Just found this 4th axis thread.
I have started a retrofit of my 3 axis cnc router and am considering adding 4th axis capability.
Found some on Ebay but cannot tell the quality or determine the electrical requirements of the steppers.
Trying to find a US distributor.

Does anyone have a good recommendation where to purchase a good 4th axis?
3 or 4 jaw lathe head 100mm opening and a tail stock?
Stepper motor with two gears and a belt drive 1:6 reduction.

What CAD CAM software is required to synchronize the 4th axis?
Looked at VCarve Pro but they only wrap a 4th axis.

Thanks in advance for the hardware and software recommendations.

Regards,
Ted

[kvom]

Got some feedback from my CAM forum and resolved a lot of issues. Seems the Mach3 Radius value in the Settings tab is ignored unless you also check the box in the ToolPath config dialog. When I did this, the engraving paths worked as they should. Now it appears that the feedrate is affected to a great extent by the A axis motor velocity and the Radius value, since when I had the velocity set to 1500 the A axis lost steps, but when I reduced it to 600 no steps were lost. However, in this test I was cutting air.

[azam1959]

these are the pp I use with fusion they should work with inventor

daniellyall, these are post processor files, right? There are four files, few words will help. Inventor come with couple of generic 4 axis post processors. thx

[azam1959]

Got some feedback from my CAM forum and resolved a lot of issues. Seems the Mach3 Radius value in the Settings tab is ignored unless you also check the box in the ToolPath config dialog. When I did this, the engraving paths worked as they should. Now it appears that the feedrate is affected to a great extent by the A axis motor velocity and the Radius value, since when I had the velocity set to 1500 the A axis lost steps, but when I reduced it to 600 no steps were lost. However, in this test I was cutting air.

kvom, vtx1800, vmax549 and SczEngrgGroup, thanks a bunch. To make sure that I get it right, I need to 1) select/click Use Radius for Feedrate from toolpath configuration and 2) from settings page on the right side I need to put distance b/w A axis and rotation axis as A rotation radius (special case, if A axis is in the center, this value will be zero) 3) start with 600 ipm for 4th axis and go from there ... I read long time ago that there was some bug in mach3 about rotation radius, any idea how i can find out if my version of mach3 has this bug fixed. i do not want to increase variable by downloading latest mach3.
thanks again and appreciate the discussion and help.

[kvom]

The radius is the actual size of the work, and is only needed if you're machining on the curved surface. When this is specified, mach3 can convert the A degree value to a linear value and thus calculate the linear distance of the G1 move. Then the feedrate tells how long that move should take and thus allows it to drive the steppers properly. That's how ti SHOULD work.I plan to do some more tests as to how accurate this is and will report back.

[kvom]

Some ore testing today. My test file consists of 3 1" long lines starting at 0,0; one horizontal, one vertical, and the other at a 45 degree angle. A G1 F15 move along each line should take 4 seconds, but each varies widely.

The other test is a 2" diameter circle centered at 1,0. The wrapping function converted this into a polyline with 102 segments, each .063" long. A G1 F6.28 should traverse the path in 1 minute. However I find it takes longer.

The wrapping specified a 3" diameter work surface. With the Mach3 radius set at 1.5 the toolpath takes 3:10. If I set the Mach3 radius to 3" it takes twice as long, and setting it to .75" halves it to 1:40. Quite counterintuitive. The motor speed of the A axis has no effect on these timings leading me to think that the set maximum isn't being exceeded. Increasing the A axis acceleration had no effect on times.

[vmax549]

AS long as you are using micro segment Lines (1000s of very small moves) instead af true arcs you are NEVER going to get full speed with ANY controller. It can't happen.

There IS a method that works in Mach3 to Do 4th axis work where Mach3 can convert itself to run the XA or YA code as XY. That way you can program directly in XY and it will wrap around the part. The advantage is it can run Arcs for the rotary motion instead of micro segmented lines. It has no problems maintaining feedrate as it does NOT have to handle the micro segmented lines. The disadvantage is you do not get a rotary toolpath shown on the screen it display as a flat plane. BUT it does machine it correctly. Haas has the same option with the axis wrapping function. That is where the idea came from.

Another note: With a 4th with a large ratio(60-90:10 You are NOT going to get the speed required to do fast rotary work. NO matter how you do it you are still limited to the speed of the slowest axis. For normal 3d 4th axis work the ratio of about 6:1 works well. THat gove you the speed you need to match the XY axis in motion.

Just a thought, (;-) TP

[daniellyall]

azam1959 sorry for no description I will try and work out what one is what

also on my router its speeds are 1250 X, Y, Z And A is 4000. 4000 is the correct speed to use as what the program say it will take to cut is about correct for how long it takes, using rotation diameter works you just have to have it bang on to the diameter of whats getting cut I have done quite a bit of A axis stuff as long as the diameter is set right I have not had a problem.

[daniellyall]

the one called mach3mill updated is a 3 axis pp it goes to work zero at start and at tool change time,

the A - This Tormach is 4th axis along x for a tormach running M3 it goes to home at start,

mach3mill with-axis is 4th axis along x the other one is 4th along y axis both goto home at start and if no tool changer home at tool change time

[daniellyall]

all the pp I posted you need to home first at a safe spot as you would anyway

[kvom]

AS long as you are using micro segment Lines (1000s of very small moves) instead af true arcs you are NEVER going to get full speed with ANY controller. It can't happen.

There IS a method that works in Mach3 to Do 4th axis work where Mach3 can convert itself to run the XA or YA code as XY. That way you can program directly in XY and it will wrap around the part. The advantage is it can run Arcs for the rotary motion instead of micro segmented lines. It has no problems maintaining feedrate as it does NOT have to handle the micro segmented lines. The disadvantage is you do not get a rotary toolpath shown on the screen it display as a flat plane. BUT it does machine it correctly. Haas has the same option with the axis wrapping function. That is where the idea came from.

Another note: With a 4th with a large ratio(60-90:10 You are NOT going to get the speed required to do fast rotary work. NO matter how you do it you are still limited to the speed of the slowest axis. For normal 3d 4th axis work the ratio of about 6:1 works well. THat gove you the speed you need to match the XY axis in motion.

Just a thought, (;-) TP

How does that work?

[daniellyall]

its just one off the ways to do it you can use notepad++ to convert Y or X to A and set the diameter then the machine will rotate around the X or Y, A acts like x or y instead of doing little moves in a straight line it moves around the line`s its the manual way of doing 4th axis work, as long as there is I and J moves or R moves it will show a round tool path.

if there`s no rotation moves it cant show a round tool path as there is nothing round to see and it cuts in little straight lines but it works all the same just slower and you can see the little lines.

the easy way is to get that tool path wrapping program the works ok slow but better than above.

look up NYCCNC on youtube he did a vid on using note pad to convert code it was not A he used but the idea is the same.

the other way is to do it in cam and set the diameter in mach this will show a round tool path every time and you just have to have the speed of the A axis set correctly.

if you run a 4th axis code and if it has a slow speed, speed up the A axis if this don't help there is something else wrong

it takes a lot of playing to work it out and how it work`s and to do it. there is a few ways to do it some just work better than others I have tried all the ways I can do it in cam now so I don't bother using any other way all I have to rember to do is put in the diameter and have the speed correct and she`s all good

you can just simulate the different ways of doing it you will see straight away if it`s not set correctly just have a play

[vmax549]

Here is where it is discussed on the Mach website.

Thinking of a new wrapper function for MAch3.

(;-) TP

[kvom]

the other way is to do it in cam and set the diameter in mach this will show a round tool path every time and you just have to have the speed of the A axis set correctly.

Are you saying that a G2 X1 A1 code will work as long as the diameter is set in Mach3?

[kvom]

I discovered that the wrapper function in my CAM program was generating incorrect code conversion.

I downloaded cncwrapper and regenerated both my test file and the engraving I initially did. Now the coordinated moves work properly and at the programmed feed rates, and the engraving elapsed time (cutting air) match the mach3 simulation of the unwrapped program. With my current settings of speed and acceleration for A, I lost no steps cutting air in either (and running at higher feed rates than I would actually use in practice).

So converting arcs to lines before conversion in cncwrapper seems to be the way to go for me.

One issue I need to be aware of is that with the axis on the left side of the table, a positive A move represents a negative Y, So I swapped the dir pin setting so that G0A10 ends up at A350 on the axis band.

[vmax549]

As a side note you cannot USE arcs with 4th axis coding so NO the code you posted " G2 X1 A1" will not work.

(;-) TP

[daniellyall]

Are you saying that a G2 X1 A1 code will work as long as the diameter is set in Mach3?

that's just a 1 move move so it will be 1 or 359 it will fault any way no R, I, J or K
a G0 X1 A180 F500 will give you a move but with nothing to see there no full rotation

you just play to work out what works M3 is good for sim and spitting out a error

when I change to M4 I am keeping M3 as my sim program

[daniellyall]

if you wont to know why you will have to ask one of the more experienced block other than one that wont post where I have been posting

I just worked out what works and does not work

[kvom]

As I posted earlier, converting arcs to short line segments in CAM and then CNCwrapper conversion gave me the results I wanted. It's clear that G2/G3 won't work natively unless the control is specifically designed to do so, and for that it also needs the radius.