z axis losing steps as I cut.

[rockaukum]

I am using fusion 360 for design and cam. I have mach3 on a cnc router table.
When I start the cut, the machine got to the correct place and cuts correctly. Tonight I tried again and here is what happened. The first three holes worked just fine. As the cuts progressed, I seemed to loose steps(?). When I watched it more closely, I see that when the spindle retracted and moved to the new drill location, instead of going down to the work piece, it raised up, slowed for the cut then moved on to the next location and did the same thing, it rose up for the cut not down!
A bit of back story as well....
I have successfully made this cut before without issue as a trial in wood. When I went to do a final cut in aluminum, the computer crashed. After the computer was fixed, I have been getting this issue. I have tried to compare various g-codes and they seem to be the same but I'm still a little uncertain if it is the computer, mach3, fusion, or me that is causing the problems.
If anyone has any information on where to start looking for a solution, please let me know!
I have set the ref all and then set the zeros at the work piece. Which I have rarely done before but I am searching for anything that may work.
If ya need any more information, please let me know.
Thanks in advance,
rockaukum

Similar Threads:

• Need Help!- Z axis losing steps?
• Problem- 770 losing steps on the z axis
• Y Axis losing steps
• Need Help!- Losing steps with the Y axis
• Y Axis keeps losing Steps

[difalkner]

You say the computer crashed and was 'fixed'. How was it fixed? Did you have to reinstall the operating system (Windows, I assume), reinstall Mach3, etc.? Were all the settings replaced by backups or created again from scratch? Are there any peripheral boards that might have been affected - ESS, etc.?

David

[rockaukum]

Hey David,
Yes the computer crashed. I had a black screen with the white cursor blinking in the upper left of the screen. What solved that issue was to remove and reinstall the ram. Took lots of reading and such but that was all it took. I started the computer in safe mode to see if there was anything else going on but was clear. I did that after each of the four ram chips were installed, one at a time. So, Nothing was changed or need to be reloaded in order for the computer to work. This computer is not on line either if that matters.
rockaukum

[mactec54]

I am using fusion 360 for design and cam. I have mach3 on a cnc router table.
When I start the cut, the machine got to the correct place and cuts correctly. Tonight I tried again and here is what happened. The first three holes worked just fine. As the cuts progressed, I seemed to loose steps(?). When I watched it more closely, I see that when the spindle retracted and moved to the new drill location, instead of going down to the work piece, it raised up, slowed for the cut then moved on to the next location and did the same thing, it rose up for the cut not down!
A bit of back story as well....
I have successfully made this cut before without issue as a trial in wood. When I went to do a final cut in aluminum, the computer crashed. After the computer was fixed, I have been getting this issue. I have tried to compare various g-codes and they seem to be the same but I'm still a little uncertain if it is the computer, mach3, fusion, or me that is causing the problems.
If anyone has any information on where to start looking for a solution, please let me know!
I have set the ref all and then set the zeros at the work piece. Which I have rarely done before but I am searching for anything that may work.
If ya need any more information, please let me know.
Thanks in advance,
rockaukum

Post the G-Code Program, there may be something in it, it could also be noise also, which would be a wiring problem, it could also so be Motor tuning that the acceleration and velocity is set to high, so something to look at

[rockaukum]

Mactec54,
The code is a .tap file and it will not accept this type of file, how do I load the code for this forum?
I did recheck the distance traveled for the z and it was good. You helped me with the vid recently, I have done several cuts since then, so I don't understand why There would be a noise issue or that the acceleration / velocity would have changed?
rockaukum
here is one part of the code, the first part. I tried to break up the code and run each portion as a separate function and had the same results

(1001)
(T15 D=0.25 CR=0. TAPER=30DEG - ZMIN=-0.0394 - CHAMFER MILL)
N10 G90 G94 G91.1 G40 G49 G17
N15 G20
N20 G28 G91 Z0.
N25 G90


(DRILL4)
N30 M5
N35 M9
N40 T15 M6
N45 S14000 M3
N50 G54
N55 G0 X1.7319 Y0.3504
N60 G43 Z0.64 H15
N65 Z0.24
N70 G98 G81 X1.7319 Y0.3504 Z-0.0394 R0.2 F13.1
N75 Y0.8524
N80 Y1.3543
N85 X1.7316 Y1.8562
N90 X1.7319 Y2.3583
N95 Y2.8602
N100 X1.7325 Y3.3633
N105 X1.7319 Y3.8642
N110 Y4.3662
N115 X1.7292 Y4.8664
N120 X1.7319 Y5.3701
N125 Y5.8721
N130 Y6.374
N135 X0.2374
N140 Y5.8721
N145 Y5.3701
N150 X0.2367 Y4.8704
N155 X0.2374 Y4.3662
N160 Y3.8642
N165 X0.2397 Y3.3621
N170 X0.2374 Y2.8602
N175 Y2.3583
N180 X0.2378 Y1.8562
N185 X0.2374 Y1.3543
N190 Y0.8524
N195 Y0.3504
N200 G80
N205 Z0.64


N210 G28 G91 Z0.
N215 G90
N220 G28 G91 X0. Y0.
N225 G90
N230 M30

[wizard]

I’d look closely at the setup files for your G-Code processor. It is always possible that invalid says information got saved at some point.

Also it is always worth having a set of hand written G-Code programs to do maintenance and diagnostics programming with. Hand written to avoid possible configuration issues with CAM software. These codes should be simple and always ran in the same way giving the same results. If not machine behavior that deviates against expected behavior can lead you to problem areas.

[rockaukum]

Thanks for the response Wizard,
I'm not sure about your first comment. I guess I'm not sure what I would be looking for or at?
As for simple code to run, I will try another code that was generated with sheetcam and see how that goes. I guess that if the same thing happens it would lead to something within the settings in mach3?
thanks again,
rockaukum
PS I am currently working on reproducing the drawing in Inkscape then code it with sheetcam to see what happens there as well.

[rockaukum]

Here is the video of what is happening. I am leaning towards this being a mach3 issue? However I am at a loss as to what may be causing this and why it has changed.
rockaukum

[m4bushy]

Mactec54,
The code is a .tap file and it will not accept this type of file, how do I load the code for this forum?
I did recheck the distance traveled for the z and it was good. You helped me with the vid recently, I have done several cuts since then, so I don't understand why There would be a noise issue or that the acceleration / velocity would have changed?
rockaukum
here is one part of the code, the first part. I tried to break up the code and run each portion as a separate function and had the same results

(1001)
(T15 D=0.25 CR=0. TAPER=30DEG - ZMIN=-0.0394 - CHAMFER MILL)
N10 G90 G94 G91.1 G40 G49 G17
N15 G20
N20 G28 G91 Z0.
N25 G90


(DRILL4)
N30 M5
N35 M9
N40 T15 M6
N45 S14000 M3
N50 G54
N55 G0 X1.7319 Y0.3504
N60 G43 Z0.64 H15
N65 Z0.24
N70 G98 G81 X1.7319 Y0.3504 Z-0.0394 R0.2 F13.1
N75 Y0.8524
N80 Y1.3543
N85 X1.7316 Y1.8562
N90 X1.7319 Y2.3583
N95 Y2.8602
N100 X1.7325 Y3.3633
N105 X1.7319 Y3.8642
N110 Y4.3662
N115 X1.7292 Y4.8664
N120 X1.7319 Y5.3701
N125 Y5.8721
N130 Y6.374
N135 X0.2374
N140 Y5.8721
N145 Y5.3701
N150 X0.2367 Y4.8704
N155 X0.2374 Y4.3662
N160 Y3.8642
N165 X0.2397 Y3.3621
N170 X0.2374 Y2.8602
N175 Y2.3583
N180 X0.2378 Y1.8562
N185 X0.2374 Y1.3543
N190 Y0.8524
N195 Y0.3504
N200 G80
N205 Z0.64


N210 G28 G91 Z0.
N215 G90
N220 G28 G91 X0. Y0.
N225 G90
N230 M30

Try using X & Y positions for all holes. We had some older controls at a place i used to work that would randomly drill out of position if we didn’t do that.

[mactec54]

Seems to be double posting again just deleted this post

[mactec54]

Mactec54,
The code is a .tap file and it will not accept this type of file, how do I load the code for this forum?
I did recheck the distance traveled for the z and it was good. You helped me with the vid recently, I have done several cuts since then, so I don't understand why There would be a noise issue or that the acceleration / velocity would have changed?
rockaukum
here is one part of the code, the first part. I tried to break up the code and run each portion as a separate function and had the same results

I don't see a problem with this program but will run it to see if it does the same thing

Post the piece of code where the problem happens

This is the same program run this and see if it all works, this I ran through Mach3 you will see the changes I made, this may not solve your problem but if this runs through then you are on the right track, you can cut and paste this into notepad then save it to a thumb drive to load into your control, if you can't find the file when you load it then select all files and you will see it


%
(1001)
(T15 D=0.25 CR=0. TAPER=30DEG - ZMIN=-0.0394 - CHAMFER MILL)
N10 G90 G94 G40 G17
N15 G20
N20 G0 Z.640
N25 G90
N30 M5
N35 M9
N40 T15 M6 (Drill4)
N45 S14000 M3
N50 G54
N55 G0 X1.7319 Y0.3504
N60 G43 Z0.64 H15
N65 Z0.24
N70 G98 G81 X1.7319 Y0.3504 Z-0.0394 R0.2 F13.1
N75 Y0.8524
N80 Y1.3543
N85 X1.7316 Y1.8562
N90 X1.7319 Y2.3583
N95 Y2.8602
N100 X1.7325 Y3.3633
N105 X1.7319 Y3.8642
N110 Y4.3662
N115 X1.7292 Y4.8664
N120 X1.7319 Y5.3701
N125 Y5.8721
N130 Y6.374
N135 X0.2374
N140 Y5.8721
N145 Y5.3701
N150 X0.2367 Y4.8704
N155 X0.2374 Y4.3662
N160 Y3.8642
N165 X0.2397 Y3.3621
N170 X0.2374 Y2.8602
N175 Y2.3583
N180 X0.2378 Y1.8562
N185 X0.2374 Y1.3543
N190 Y0.8524
N195 Y0.3504
N196 G80G0Z0.64
N198 G0 Z2.
N199 G90G53G0 X0. Y0.
N200 M30
%

You can save the file in MS word as Text your file or even Note pad, the program can have a end name as Text this will run on your control as well, You can also just cut and paste it into your post

[vmax549]

Thee are quirks in teh G81 drill cycle that can show up from time to time. Try changing to another drill cycle like G83 and retest.

Just a thought, (;-) TP

[he1957]

N10 G90 G94 G91.1 G40 G49 G17

N20 G28 G91 Z 0.

Remove the G91.1 and G91 codes and see if that helps. Also the tool length compensation (G43+) may be being added to the offsets since it's in incremental mode.

[mactec54]

N10 G90 G94 G91.1 G40 G49 G17

N20 G28 G91 Z 0.

Remove the G91.1 and G91 codes and see if that helps. Also the tool length compensation (G43+) may be being added to the offsets since it's in incremental mode.

They are already removed in the code I posted, and he is not using incremental mode it's programed as it should be in absolute

[rockaukum]

So, with my frustrations check, I decide to reinstall mach3 and establish a new profile. I copied via screen captures to record the input information. Loaded the information into the profile and took the desktop back to the shop. I did a trial with out the machine connected and it looked like it was working, DRO's moving in the correct direction... I hooked up the machine to the computer and nothing happened! Too frustrated to continue so I packed it in for the day. I spent the morning reading the manual to see If I can figure this out that way. I also tried to run your code (mactec54) and had no luck and had to reenter the values of the code as when I copied it via text edit (Mac) and view it with word it was weird. So I cleaned it and saved the file. Needless to day it did not work, still.
Today I went to the shop and loaded the original profile and ref all, set work coordinates and tried an air cut and it appeared to work just fine? I set the zero on the stock and started again, Again it (your code) worked just fine? This is leading me to think it was the gcode produced by fusion360. Thinking that I have cut this whole code before and only made change to the code and that was the peck feature (drill? in fusion) that may have caused this whole issue? Anyway, I'll try and run the program that Fusion created without the pecking and see how that goes.
While I'm here, How do you change the g28 settings so when a cut is finished, the gantry will move to a different location instead of machine 0,0,0? The way the machine sits in the shop, I'd like to have it park in the upper right corner (when standing at 0,0,0, lower left of the table)
Many thanks for helping out!
rockaukum

[mactec54]

So, with my frustrations check, I decide to reinstall mach3 and establish a new profile. I copied via screen captures to record the input information. Loaded the information into the profile and took the desktop back to the shop. I did a trial with out the machine connected and it looked like it was working, DRO's moving in the correct direction... I hooked up the machine to the computer and nothing happened! Too frustrated to continue so I packed it in for the day. I spent the morning reading the manual to see If I can figure this out that way. I also tried to run your code (mactec54) and had no luck and had to reenter the values of the code as when I copied it via text edit (Mac) and view it with word it was weird. So I cleaned it and saved the file. Needless to day it did not work, still.
Today I went to the shop and loaded the original profile and ref all, set work coordinates and tried an air cut and it appeared to work just fine? I set the zero on the stock and started again, Again it (your code) worked just fine? This is leading me to think it was the gcode produced by fusion360. Thinking that I have cut this whole code before and only made change to the code and that was the peck feature (drill? in fusion) that may have caused this whole issue? Anyway, I'll try and run the program that Fusion created without the pecking and see how that goes.
While I'm here, How do you change the g28 settings so when a cut is finished, the gantry will move to a different location instead of machine 0,0,0? The way the machine sits in the shop, I'd like to have it park in the upper right corner (when standing at 0,0,0, lower left of the table)
Many thanks for helping out!
rockaukum

Yes if the word changed it then it was in a different format before you open it set up the save as type at the bottom of the word window Notepad should work as well, the program I posed run in Mach3 may be 50 times without a miss

You want to change your post processor to get rid of the G28 used in your program like I posted G28 is incremental and if you don't have a G90 after it's use you have a good chance of crashing, so it is best not used

To get your machine to go where you want it

G80G0Z2.0 ( G80 only used if you are doing a canned cycle Drill Etc G80 cancels the Canned cycle and the Z axes moves up 2" or any number you want it to )

G90G53X______Y_________ ( to where ever you want it to move to )

M5

M30
% ( Don't forget this at the top of your program and the End of the Program )

[m4bushy]

.