Machine/Program not running correctly (Resolved)

All things related to Centroid Oak, Allin1DC, MPU11 and Legacy products

Moderator: cnckeith

Post Reply
Jones Outdoors
Posts: 9
Joined: Tue Oct 06, 2020 7:57 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: A900938

Machine/Program not running correctly (Resolved)

Post by Jones Outdoors »

Machine: Alliant Knee Mill
Control: All In One
CAD/CAM: Fusion 360

Hey guys,
Been working on getting my mill up and running. Got All In 1 installed and everything responded as it should. Now I am trying to run a program and actually put it to work. I'm a green horn so I know I'm missing something.

The Problem: I have a facing operation as the first operation of my program. After starting the program and when starting the facing operation, the Z axis comes down and limits out. I only have about 3.25 inches in my Z axis travel before it hits the limit. I have the knee up so it should only have to move about 2 inches to the work top. Also, it appears that it is not starting the facing operation on the material but out in front of it. It limited out so I can't tell which way it was going to go. I am dry running this with the vice off so I would avoid any crashes and such.

I have set all my tools heights with a reference tool on top of my vice not the material. It is about an inch longer than my longest tool. I used an edge finder to set up my material.

I should mention that I only have one limit switch per axis right now. I had a professional install the All in One who is familiar with doing this. I am not an electrician but I do remember him telling me that he had to use jumper wires to make the switches work. I think he said it would not know which limit was tripped so I would be dead in the water until hitting the E-Stop and manually moving the machine off the switch. I didn't think that would cause any issues since I wouldn't be working on anything that would use up that much of the table. I have not been able to set a permanent home because of this. I have to crtl S every time I start up the machine. I'm ok with this unless this is what is causing my problem. As far as it appearing to not start in the correct location, it may be something in Fusion. I have my WCS set on the same corner where I use my edge finder. Not sure if that is the way to do it or not. Any help would be most appreciated. I am sure I will be back once I get past this little issue with another one or two.

Thanks
Bryan
cncsnw
Posts: 1971
Joined: Wed Mar 24, 2010 5:48 pm

Re: Machine/Program not running correctly

Post by cncsnw »

Please post a current report.

It is not clear whether by "limits out", you mean that the Z axis moves high enough or low enough to actually trip your Z plus and/or minus limit switch (and hence give you a "407 ... limit tripped" message); or whether you mean that you get a "907 ... axis travel exceeded, line ..." message.

It is likely that your limit switch setup could be significantly improved. If you have only one switch per axis (designed to trip at both ends of axis travel) you would be best served by wiring that switch to only one limit input: the one in the direction you would like to home to. You would then rely solely on software travel limits to prevent overtravel in the other direction. The other limit input would be defeated with the DIP switches (or a wire jumper if you prefer). Done that way, you would be able to automatically and consistently find home.
Jones Outdoors
Posts: 9
Joined: Tue Oct 06, 2020 7:57 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: A900938

Re: Machine/Program not running correctly

Post by Jones Outdoors »

Ok. I have found a rookie mistake I made but I still have an issue. I found that I used the wrong tool # when I was setting the part height. The issue that I still have is the Z axis is still coming down too far. It is not hitting the limit switch but it is coming down about an 1.25 inches too far. It's acting like it has lost the xzy zero the best I can tell or at least the z zero. I can manually move the axis to these zero positions and all appears to be in the correct location. When I start the program the Z axis just goes where it wants to. I'm sure that it's just me doing something wrong or our of order or something. I am attaching a report that hopefully could show any issues. I will get to work on figuring out how to work the limit switches like you mentioned or just buy some more and have two switches on each axis. I would rather go that route.
Thanks for your help
Bryan
Attachments
report_0008DC111213-1111202495_2021-03-15_17-44-56.zip
(4.81 MiB) Downloaded 9 times
cncsnw
Posts: 1971
Joined: Wed Mar 24, 2010 5:48 pm

Re: Machine/Program not running correctly

Post by cncsnw »

When it "comes down about 1.25 inches too far", does the Z axis DRO show the position in the program, that it is supposed to be at? Or does it show a position 1.25" lower than what you put in your program?

Say, for example, that you write a program that uses work coordinate system #1 (G54); loads tool #3 (M6 T3); turns on tool height offsets for tool #3 (G43 H3); then moves Z to -0.500" (G1 F__ Z-0.500).

If the program was written correctly and the control is functioning correctly, then at the end of that Z-down move, the status window will say "T3 H3", the top left corner above the DRO will say "WCS #1 (G54)", and the Z line of the DRO will say "Z-0.5000".

If, in that case, the tool is lower down than you intended or expected, then you probably made a mistake either in setting your part zero, or in measuring your tool height offset. If it was a mistake in setting part zero, then each tool, when called up with its appropriate offset, would go too deep. If it was a mistake in measuring the tool height offset, then it is possible that only that one tool would go too deep.

Perhaps next time it happens you can pause it (Feed Hold) while it is at this excessive depth, take a picture of the screen (the whole screen, not a close-up); and post that picture here along with a copy of the CNC program file that was running.

If instead the DRO position shows, for example, "Z-1.7500" when you thought you programmed it to go to -0.500, then chances are the error was in the CAD/CAM software when you described your toolpath.

Does your CNC program always use matching T and H numbers?
Does your CNC program explicitly call up one work coordinate system or another?
If so, are you setting your part zero in that same work coordinate system?
Dave_C
Posts: 599
Joined: Wed Nov 15, 2017 8:25 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none
Location: Springfield, MO. USA
Contact:

Re: Machine/Program not running correctly

Post by Dave_C »

I have not been able to set a permanent home because of this.
Hum, if the machine does not know where home is, how does it know the extent of the soft travel limits?

Sure you can move it to marks and set home from there and that will work. Very easy on the X-Y axis, but if you are not doing something similar in the Z axis, it does not know where it is.

With all tools set from one reference point, you still need to set the Z axis to a zero point.

Here is how I do it for my knee mill:

I lower the quill to 1" (that give me clearance to step over clamps) I set my part zero there and then I call my first tool and raise the knee until the tool tip touches the part.

And since my system is an R8 collet system, there is no way for me to get repeatable tool lengths. So all tool lengths are set to "0" in the tool table. Each time I change out a tool I let the machine go back to the G28 position, measure the distance from the tool tip to the table with a gauge that sits on the table, change tools and then raise or lower the knee until the gauge I used reads the same.

That way my program zero never needs to change!

Dave C.
Grizzly G0678 Mill ,CNC conversion with Acorn. G4004G Lathe, Mach 3 conversion to Acorn.
Jones Outdoors
Posts: 9
Joined: Tue Oct 06, 2020 7:57 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: A900938

Re: Machine/Program not running correctly

Post by Jones Outdoors »

#cncsnw
Ok I'm getting close. With all my superior intelligence I think I'm going to make every rookie mistake possible so I can get them all out of the way. I found that some how I had my tools numbered differently in Fusion than what I had in Centroid and therefore seems to explain the Z going so deep. I fixed that and now it appears to cutting about .1875 in. too deep. This could be due to the way I have it set up in Fusion or tool offset setup. It is not obvious to me yet but I'm poking around hoping it will jump out at me. When I start the program it does take the Z to zero (picture attached) but still a little deep. Code is posted also with hopes you may identify something that may not be correct. I appreciate the way you responded as I just learned a tremendous amount. I now need to understand it. I'm getting there. I really appreciate you taking time to help me out with this.

Does your CNC program always use matching T and H numbers? Good question. This is my first run at running a program. I will pay attention
when I get some success and get to run a few more programs.
Does your CNC program explicitly call up one work coordinate system or another? Same answer as above
If so, are you setting your part zero in that same work coordinate system
? Is this good or bad if it happens like this and what to do if bad?


#Dave_C
Thanks for the response. When I get far enough along I may have to do what you do to keep zero. I'm still learning and I have plenty still to go.

Thanks all
Bryan
Attachments
Code.JPG
.1875 too deep.jpg
Z at zero.jpg
cncsnw
Posts: 1971
Joined: Wed Mar 24, 2010 5:48 pm

Re: Machine/Program not running correctly

Post by cncsnw »

That pretty well narrows it down to a setup issue, either in setting the Z axis part zero, or in measuring the tool height offset.

Your program correctly calls up H6 when it is cutting with T6. Your control moves to Z0.0000, using that height offset when told to do so.

Do other tools that you set up in the same batch also go too deep? By the same amount, or by varying amounts?

One thing you can do after you have completed your setups, before you run the job, is to position X and Y off to the side (as in your picture above) then use MDI to activate a tool offset and move Z to part zero.

For example, you could load tool #3 in the spindle, and use MDI to run "G43 H3 G0 Z0", and see where it ends up.
Then you could load tool #4 into the spindle, and run "G43 H4 G0 Z0", and see where that one ends up.
... and so on through the tool list.

It is not necessary to run an M6 or change the T number when doing that. For the purpose of Z axis positioning, the G43 and the H code are the only things that matter.
Dave_C
Posts: 599
Joined: Wed Nov 15, 2017 8:25 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none
Location: Springfield, MO. USA
Contact:

Re: Machine/Program not running correctly

Post by Dave_C »

I must be missing something here because the OP says he has an Aliant knee mill.

So with just 3 1/2" of travel I'm guessing that is the quill travel and if he is setting tool lengths, how is he getting them back in the machine to length.

Is this an R-8 machine or does it have Cat-40 tool holders. (I don't know the machine)

Dave C.
Grizzly G0678 Mill ,CNC conversion with Acorn. G4004G Lathe, Mach 3 conversion to Acorn.
Jones Outdoors
Posts: 9
Joined: Tue Oct 06, 2020 7:57 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: A900938

Re: Machine/Program not running correctly

Post by Jones Outdoors »

Good news. I have this thing running correctly so far. I went back and remeasured all my tools then re-set up my tool offsets and I was able to get the facing operation looking good. Didn't have time to go any further but it visually it looks it will all line up. I really appreciate all the help. I'm still learning and when talking to someone who knows what's going on really helps me put together all the things I don't fully understand yet. I'm sure I will be back needing other help soon.

#Dave_C
I have both R-8 and either Cat 40 or 30 or something else - pic below. I do have room to get the tools in although if I were to get any longer tools I see where I could have issues. Also I used them with one of my short tools the short tool may not make it down to the material. I already see that I am already approaching maximum extension of my Z with a couple of my short tools with where I have the knee now. Most likely I will have to crank it up couple of turns to give me a little more confidence. I really appreciate your input as you seem to have a good visualization of my machine and the issues that can come up. Anyway thanks for all the help.

Bryan
Attachments
holder.jpg
martyscncgarage
Posts: 7883
Joined: Tue Mar 28, 2017 12:01 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: Yes
CPU10 or CPU7: Yes
CNC Control System Serial Number: none
Location: Mesa, AZ

Re: Machine/Program not running correctly

Post by martyscncgarage »

Jones outdoors,
It looks like an NMTB 30 holder, what does it say on the otherside?

Have you taken the time to watch Centroid CNC's Mill Training videos on YouTube? Well worth watching both of them!
Glad you are on your way....
Marty
Reminder, for support please follow this post: viewtopic.php?f=20&t=383
We can't "SEE" what you see...
Mesa, AZ
Post Reply