Crashing into work

Hello All. So I built a 3 axis machine and it's been working great. I've cut several projects without issue. So I'm working on upgrading the spindle again to a Makita router. I made a mounting clamp for the router using Fusion360. I plan to cut this from an aluminum block which is 44mm tall, 110 x 152. I can only cut to 37mm. I plan to cut the clamp from the remaining block with a band saw.

I set the system in motion and the spindle is crashed into the side of the work piece. Several more attempts with the same result each time. I tried using a block of wood at just about 20mm thick. No problem. I replace the aluminum block and again it crashes. I am homing and then I do a touch off. X, Y then Z. Everything looks fine on the screen and then it crashes. It's trying to get to the first operation by moving through the work piece. Please... why?

I'm not sure what other information might be required here. Sorry if I missed something.



Thank You,
John

The post is doing a G28 to Z0 so if anything is in the way and parameters are not set it will move regardless if stock is in the way.

I would modify the post and fix that. Get rid of the G28 move and go to a safe Z.

Just my thoughts.

I see this too looking at the file in editor, but i don't know what G28 is. I've read about it here linuxcnc.org/docs/2.6/html/gcode/gcode.html, but what the heck is 5161-5166 and where did the paramters stored there come from?

So you want me to remove the line with G28 G91 Z0? Do I then jog to the x y start position above the location to be cut and then run the program?

Also when i said the spindle is crashing into the work I should have been a bit more accurate in my description. It's about 5mm of the end mill. So if I start the machine at x-100, y-100 and z50 then click run on the program it drops the spindle to like z-5 and drives into the side of the work piece. hopefully I have better described what i'm experiencing. why is fusion360 putting out code that drives through the material on it's way to the first cut coordinates?


Thank You,
John

Bumbino wrote:

I see this too looking at the file in editor, but i don't know what G28 is. I've read about it here linuxcnc.org/docs/2.6/html/gcode/gcode.html, but what the heck is 5161-5166 and where did the paramters stored there come from?

So you want me to remove the line with G28 G91 Z0? Do I then jog to the x y start position above the location to be cut and then run the program?

Also when i said the spindle is crashing into the work I should have been a bit more accurate in my description. It's about 5mm of the end mill. So if I start the machine at x-100, y-100 and z50 then click run on the program it drops the spindle to like z-5 and drives into the side of the work piece. hopefully I have better described what i'm experiencing. why is fusion360 putting out code that drives through the material on it's way to the first cut coordinates?


Thank You,
John

I'm not comfortable with th3e G28 moves. I would put a G0 G53 Z0, that way first thing it does even before starting spindle moves to home position on the Z.

Now It seems it is cutting above Z0 which I don't understand. Are you setting Z0- to stock bottom or on top of the part?

when I do the manufacturer setup in fusion i select the 'model orientation' in the WCS then 'stock box point' in origin. I then select the dot on top of the material at the x0 y0 corner. In the stock setup I select 'relative size box' and add 0 to top and side offsets.

The file that I attached worked flawlessly using shorter material. Even with z touched-off at the top of the shorter material.

Most of my earlier projects would work in the way you described as i recall. No matter where my spindle was, when I clicked start the spindle would raise up to my highest z posotion, then xy into position before lowering z. This is not working that way. I've compared this Gcode to those earlier which worked, but i get lost with the the various G28 or G90 type movements. I don't know what they are the and user manual .... i dunno.... i guess it confuses me more.

Thank you,
John

Make sure you don't have any values in your tool table. I once had an offset get added to the tool table somehow and in my case it kept cutting air above the part.

How do you have this set in your .ini ?
TOOL_CHANGE_QUILL_UP = 1 - The Z axis will be moved to machine zero prior to the tool change when the value is 1. This is the same as issuing a G0 G53 Z0.

I just checked the tool table. I do have around 20 tools in there. Should I remove them all? I thought they had to be there. None of them are the tool that i'm using now, is that a problem? I'm guessing it is. Tallest thing I've cut so far. I looked at the ini file and didn't notice this TOOL_CHANGE_QUILL_UP anywhere.

Thank you,
John

All you need to do is, at a safe X Y Z position execute G28.1
Then at beginning and end of your program the G28 moves go to this position. Or get rid off the lines with G28, also at the end and enter a safe Z position. Tooltable is irrelevant, because T1 is selected, but no M6 or M61 Q1 done. So you work without T number in spindle, which is no problem with a single tool job and touch off XYZ to G54.
And add G64 P0.005, the G2 and G3 moves will get more accurate

andypugh wrote:

Bumbino wrote:

I just checked the tool table. I do have around 20 tools in there. Should I remove them all?

I think that the advice was just to make sure than none of them have a spurious X or Y offset in them. And that the Z lengths are all correct.

Yes, that was the reason. I also use F360 and use one tool per file and touch off the tool on a touch-plate sitting on top of the stock. My tool table usually has zero values in all fields. One time I somehow got values on the tool length and that caused problems. When F360 specifies a tool number, that tool number needs to be in the tool table and since we touch the tool off on the stock the tool length needs to be zero.

So to answer the question "Should I remove them all?" I would say no. Just make sure the tool lengths are all zero. This works for me and I am by no means any kind of expert on this so please feel free to correct me if needed.

John