Not equal corners radius

Hello,

So I have a problem, I've recently bought chinese manufactured CNC machine (BCAMCNC) and everything is perfect with it except that when i try to mill a square, the outside corners of it are not equal when milled even though in the sketch of aspire they're perfectly equal. I;ve tried changing a few params in the machine, experimented with aspire by trying to save the code in different formats, but result is the same. One corner is milled perfectly, but the other ones have a bigger radius. Do you have any ideas how could I fix that?

I've attached some pictures to understand the problem better.

Thanks in advance :)

Can you post the g-code for the moves?

%
:7777
N20G91G28X0Y0Z0
N30G40G17G80G49
N40T3M06
N50G90G54
N60G90G71
N70G43Z33.010H3
N80G00X0.000Y0.000S19700M3
N90G00X53.000Y53.000Z33.000
N100G01Z9.000F1500.0
N110G01Y347.000F9000.0
N120G01X347.000
N130G01Y53.000
N140G01X53.000
N150G00Z33.000
N160G28G91Z0
N170G49H0
N180G28X0Y0
N190M30

control system syntec 60w-e

Some industrial machines will have a "feature" in the control thats looks ahead and anticipates a corner and will insert a radius move around the corner to smooth the transition from one vector to the next. You won't see it in the code. When it works its great, but when it doesn't, it can drive a machinist nuts. In the case of a closed square loop or the like, the point where the cut starts and stops will be square, but the balance of the corners could be rounded. Hard to imagine a hobbyist machine having this issue, but possibly.

If Aspire has a trace command (the tool follows a centerline geometry), you may want to try that to see if it will "correct" the problem. The trace command carries the tool past the corner of the cut before it changes direction to cut the next vector. Hope this helps.

...without knowing your machine programming language format...I'm guessing what you need to do is program an "Exact Stop" code. G09/G08 or G64/G61 or it maybe called Accel/Decel/Ramp.
https://www.cnccookbook.com/g61-g64-...cise-position/

The sloppy way would be to add a wait/pause at the end of each straight cut to allow settling time on the motion axis.

After adding G61 the corners are milled perfectly! But now (with G61) when I try to mill a smaller or bigger circle it's running about 10 times slower and the machine is running very twitchy.

That's the down side of G61; it stops at the end of every vector until it gets removed. It is a modal call. You need a G64 after your hard corner stops to cancel it out where you don't want it.

Maybe you still have an opinion on why the angle is uneven?

Quote:

---

Originally Posted by MARV

Some industrial machines will have a "feature" in the control thats looks ahead and anticipates a corner and will insert a radius move around the corner to smooth the transition from one vector to the next. You won't see it in the code. When it works its great, but when it doesn't, it can drive a machinist nuts. In the case of a closed square loop or the like, the point where the cut starts and stops will be square, but the balance of the corners could be rounded. Hard to imagine a hobbyist machine having this issue, but possibly.

If Aspire has a trace command (the tool follows a centerline geometry), you may want to try that to see if it will "correct" the problem. The trace command carries the tool past the corner of the cut before it changes direction to cut the next vector. Hope this helps.

---

Can you tell us more about that?

What we're talking about here is using the tools effectively that are available to us. The more versatile CAD/CAM software packages will offer a variety of options for completing a certain task, but you need to know what those options are and how to use them before they can be a benefit. Over time you'll find that each package has certain shortcomings that may affect your work on aa given machine. Its the creative use of the software and the knowledge of how certain G code "edits" can be made to circumvent "issues" at that machine. After all, its the control that will have "the last word" as to how the code is interpreted and applied to the tool path.

Knowing that your setup may add an arc at the end of a straight line cut as a means of avoiding a hard stop (and instead maintaining a smooth cutting speed), but executing the move poorly (resulting in a rounded corner), you may want to edit the code with a G61 (a modal call) to avoid the issue. Beyond that, if there are curves and arcs to be cut, you'll want to negate the modal call so the machine will continue to move smoothly. To know more about this, you really need to study the reference mentioned earlier (https://www.cnccookbook.com/g61-g64-...cise-position/). And know that these calls can sometimes have disastrous results if not applied carefully.

Quote:

---

Originally Posted by MARV

What we're talking about here is using the tools effectively that are available to us. The more versatile CAD/CAM software packages will offer a variety of options for completing a certain task, but you need to know what those options are and how to use them before they can be a benefit. Over time you'll find that each package has certain shortcomings that may affect your work on aa given machine. Its the creative use of the software and the knowledge of how certain G code "edits" can be made to circumvent "issues" at that machine. After all, its the control that will have "the last word" as to how the code is interpreted and applied to the tool path.

Knowing that your setup may add an arc at the end of a straight line cut as a means of avoiding a hard stop (and instead maintaining a smooth cutting speed), but executing the move poorly (resulting in a rounded corner), you may want to edit the code with a G61 (a modal call) to avoid the issue. Beyond that, if there are curves and arcs to be cut, you'll want to negate the modal call so the machine will continue to move smoothly. To know more about this, you really need to study the reference mentioned earlier (https://www.cnccookbook.com/g61-g64-...cise-position/). And know that these calls can sometimes have disastrous results if not applied carefully.

---

But it's not possible .. My works have both straight and round corners and every time I write G61 or G64 code, I think it will take a lot of time.

Quote:

---

Originally Posted by Topgirda

After adding G61 the corners are milled perfectly! But now (with G61) when I try to mill a smaller or bigger circle it's running about 10 times slower and the machine is running very twitchy.

---

...maybe a good reference that may help is the way Linux G code handles G61/G64 Path Blending (see link below) most Fanuc, etc machine are usually about the same format. Try just adding G64P.015 or some P value of your choice for speed testing.
https://linuxcnc.org/docs/html/gcode...html#gcode:g64

Quote:

---

Originally Posted by machinehop5

...maybe a good reference that may help is the way Linux G code handles G61/G64 Path Blending (see link below) most Fanuc, etc machine are usually about the same format. Try just adding G64P.015 or some P value of your choice for speed testing.
https://linuxcnc.org/docs/html/gcode...html#gcode:g64

---

Thanks I will try it

...programmers make the rules ---control the programs. software Rule 101