Boss/BobCad 21

[frog]

I am having problems cutting circles ya just round circles, I am using version 21 I can do text perfect anything square, great when I get it to cut a circle it only cuts half of it, then stops, I have made sure in the setup I am using incremental and also selecting G91 to start, I had it work correctly a couple of times then when I went back the machine changed its mind and decided to do different. Can anyone help me setup my Boss5 with BobCad please? Awesome product they are very customer friendly however I believe that the tech service department is over loaded, I would appreciate it if someone could help me.

[HuFlungDung]

What does your sample code look like?

Some of those older cnc's could not cut a complete circle with one command, so the post processor needs to be set to output either 2 or 4 commands for a complete circle. 4 commands means one arc for every quadrant, and any controller will execute that.

You might also consider that switching back and forth between incremental and absolute can cause problems. Most would recommend that programming be done in absolute mode, and that the post processor be set to output arc end coordinates to match absolute mode and leave it alone when you get it working.

Reserve incremental programming for short subroutines.

[cabledude]

Hi Frog-
I agree with Hu regarding absolute coordinates. Out of the hundreds I've written for my BOSS 5 & 6, only a couple use incremental, and those can be problematic, especially if you have to stop the program midstream.

In order to get the BOSS 5 to do a circle using one line of G2 or G3 is to invoke G75 prior to the G2 or G3 lines. The manual says:

"G-75 Multi-Quadrant Circular Interpolation (restricted to XY plane)
G75 permits an arc of up to 360 degrees to be generated in a single block of input data without deceleration taking place at the quadrant cross over points."

I always use the absolute I & J coordinates as well.

Just use something like this:

N100G75G90
.
.
.
N140G0X1.000Y1.000Z.050
then some Z move, presumably
.
N160G2X1.000Y1.000I0J0F30

This will cut a (clockwise) circle starting at X 1.000, Y 1.000 with the center at X0 Y0. This example has the same start and finish point.

The F75 is modal, that is, once invoked, the machine will use it for all circle moves within the program.

Give the G75 a try and see if it works with your program.

Rob

[frog]

I understand that there is a quadrant issue with the Boss 5, however the question that I have is this, I can cut text perfect and I do not have to do anything special, in the text I can cut circles, it works perfect, however when I go to doing a circle, a simple circle it goes nuts. I did try your suggestion I drew the circle in 4 quadrants then set the tool path as per four individual quadrants, and then there was a problem it cut an out of round circle, I did declare G75G90 at the start of the code, I am pulling out my hair.

[cabledude]

Hi Frog-

First of all, I'm assuming that your Bobcad is feeding your G code into a box-stock BOSS 5. I have both a BOSS 5 and 6, and I have written hundreds of pgms for both. The biggest learning curve for me was learning how these machines think. Back in the early 80's (yeah, I'm old) I had a problem with an intricate part that required over a dozen intersecting radii. Machining this part for production justified the purchase of our first CNC machine. I spent many nights trying to figure out (using trig...remember that?) these points of intersection with no luck. The machine seemed to just go off on a tangent...literally. I finally gave up and called on a friend who worked at Bridgeport Machines (my shop is in Bridgeport). He put the drawing through his CAD system and gave me a punch tape (everybody uses those, right?) of the cutter path. The important thing I learned is that the finish point of a circle needs to be exactly the same as the starting point, to four decimal places. Even though the BOSS 5 steps at .001, it thinks (computes) to .0001. Even if not a full 360, you need to be accurate with your start point, end point and radius.

My point is, make sure you know exactly where your machine thinks it is (within .0001) when you call for a G2 or G3 move, and make sure the X & Y finish point you call out is identical (for a full 360). Don't try to put any Z moves into the line, either. Also, make sure your I and J are accurate to within .0001.

I have never had a problem with a simple circle, say starting at X1.000 Y0 I0 J0 and going 360. It's only when the circle starts at a point OTHER than the called out finish point.

As Hu previously pointed out, seeing your code might help us figure out what's going on.

I have a bunch of pgms that use cutter comp. If you think circles are fun, just wait 'til you try to add this to the mix! Fortunately, I use the machines for limited production, so once I get the program right, it's on cruise control. (until the drive transistors blow)

Keep us posted and although I still have my hair, I'm prematurely gray from the BOSS experience. :-)

Rob

[frog]

I finally did it, I was so surprised what it was, I have done serial development and would never have guessed in a million years what it was, I changed the comm setup from 7.e.1 to 8.e.1 that fixed the problem it now cuts complete uninterrupted circles machine works great, I would have never thought, due to the fact that it did text perfect, I did load with a port sniffer program, and when I used 8,e,1 it was great, when I used 7,e,1 it had some garbage in it, now I am off to the races. Thanks for all the help.