[mpq1969]

I am very new to working with a CNC and acquired a homemade system from an associate to work with and learn. I usually do 2D stuff on it and find it fun but thought I'd try my hand at engraving. The problem is that the depth of the cut seems to change, it gets deeper, with every letter I engrave. I'm using Mastercam X3 for the engraving and Mach3 from Artsoft to run my machine.
The engraving is pretty simple so I didn't expect any issues. I chose "contour" for the toolpath and "window" then selected the text.
I've done many 2D things before without this issue so wondering why it happens when I'm engraving letters.
Any help is appreciated. If needed I can attach G code also
Image attached showing what the engraving did. I stopped it mid cycle since it obviously was having issues.

[C*H*U*D]

Since it's wood, are you sure it's flat? I see the groove on top, so I'm assuming it is but figured I would ask anyway. Also, it's not bowing under clamping pressure is it? I would check the Z height at each end of the lettering to rule out any issues with the workpiece.

While it's running, do you see the Z changing on your readout?

[Claude Boudreau]

One possible explanation could be the motor loosing steps going up and not going down with gravity helping.
Possibly a motor tunning problem , i would try slowing down the speed and acceleration on the Z axis.

[mpq1969]

Since it's wood, are you sure it's flat? I see the groove on top, so I'm assuming it is but figured I would ask anyway. Also, it's not bowing under clamping pressure is it? I would check the Z height at each end of the lettering to rule out any issues with the workpiece.

While it's running, do you see the Z changing on your readout?

You are correct. The groove on top was a manually run line to verify flatness of the piece and the co-planarity between the cutter and the work surface. I am actually on an area of my table that I put a small sacrifice board down (about 8" x 10") and then lapped it into co-planarity with a flat end mill. This is because I know there is a small issue of co-planarity between the cutter head and the work surface.
The line shows there is little issue in this area.
The wood was mic'd in four locations around and all measurements were very close to each other. Nothing along the lines of what the actual engraving is showing.
During the actual machining I was watching the code and all the bottom limits hit -0.007 exactly where it should be but the actual V tool was clearly well below that mark.

[mpq1969]

One possible explanation could be the motor loosing steps going up and not going down with gravity helping.
Possibly a motor tunning problem , i would try slowing down the speed and acceleration on the Z axis.

Thank you for this suggestion. I'll try slowing down the speed and acceleration and see if this works. I'll post back if successful.
Right now I have the feed and plunge rate at 21.7 (as a newbie I'm only assuming that is mm/sec, am I correct?)

[mpq1969]

Unfortunately slowing down the feed, plunge, and retract rates to less than 1/4 of their original settings only seemed to increase the rate at which the V tool went deeper.
Like I said I know the machine itself has a co-planarity issue (it is a homemade machine) but I don't usually have this big of an issue in cutting out 2D parts in such a small area. I've even made lithophanes out of corian in this same exact area and the variance in the depth is so small it doesn't affect the part.

[Superman]

Put up the NC code
- we can check to see if the Z depths in the program ( this should eliminate any Mastercam or NC code issues. )

When you set your tool, to the top of the job, I assume it (work surface) is Z zero
- run the program
- put the tool back to Z zero.........Is the tool at the same height ?.......if not, it may point to a machine issue ( tool moving out, Z axis losing itself

[mpq1969]

Here is the code.

I do set Z zero at the top of the piece I'm working on. In this case it was the top of the oak board I was engraving.
I'll try to run the program again, this time letting it finish through the entire thing, then re-check to see if Z zero is still at the top of the oak board or if it moved.

[Superman]

Looked at the NC file

all cutting was done at Z-0.007 & then at Z-0.008
- this is NOT showing any reason for the deeper cuts in your part

Board flatness is also eliminated, for the reason that there is a deep cut near the shallow cut

Look for :-
- tool moving out of the holder
- Z axis losing itself

On a side note:-
your program has

N5060 G0 Z.25
N5062 M5
N5064 G91 Z0. <--- does the machine move anywhere when these are executed
N5066 X0. Y0. A0. <--- ditto
N5068 M30


change to
N5060 G0 Z.25
N5062 M5
N5064 G91 G28 Z0.
N5066 G91 G28 X0. Y0. A0.
N5067 G90
N5068 M30

or
N5060 G0 Z.25
N5062 M5
N5064 G53 Z0.
N5066 G53 X0. Y0. A0.
N5068 M30

G91 G28 is...return to machine home
G53 is....... use the machine coordinate system ( not the G54 )
check that these are usable in your manual

[bushwakka]

I've previously had issues with the following.
* slip on the coupling between the motor and ballscrews.
* the cutting bit being pulled out of the collet (up cut bits)
* the spindle moving in its bracket.


Sent from my iPad using Tapatalk

[mpq1969]

Thanks Superman I'll try to go with the G91 and G28 codes and add those in.
The G28 codes are automatically there but in the past I've had issues with machine zero and had the end mill plunge into my parts at the end so I removed the G28 to stop that from happening.
I wasn't sure how to change machine home but I think I've fixed that so I'll leave the G28 in there this time and test it to make sure machine home is correct.
I also don't think it is the tool itself slipping (cutter too loose and moving inside the collet) because it is consistently cutting deeper and not more shallow. I would expect the opposite effect of what I'm seeing if the V tool was actually becoming loose in the collet.
To answer your question about the machine moving anywhere at the end, without G28 it simply finishes the part and then Z's up only from where it ended. Again, that was the safest way for me to avoid having it plunge into my part and cause problems.

[mpq1969]

Thanks Bushwakka. I'm not sure about the coupling between the motor and ballscrews. If that was a problem wouldn't it be consistent with all projects? I only have this issue on engraving. When I cut out 2D parts I don't see the cutter gradually lowering itself into the part.
For instance if I cut out a simple square that requires 5 passes to go completely through the material the cutter doesn't appear to go lower than the NC code shows each pass. Again, only on engraving do I see this phenomena

[hub]

Check running with a dial indicator that the table (and part) is straight. Looks to me like it's not.

Hub

[mpq1969]

Hub,
I'll see if I can get hold of a dial indicator and check the actual variation from one side of the part to the other

[bushwakka]

I would try something like
1. Engrave a line at z=1
2. Cycle z axis up and down 50 or so times.
3. Engrave a line at z=1, right next to the other line.
As the bit hasn't been cutting, you should be able to rule out issues with the bit, collet, etc.

If it is different, you are missing steps, or slipping coupling on the shaft.


Sent from my iPad using Tapatalk

[minicncuser]

I would try to set my feed plane and retract to the same height and both at absolute shut off clearance. I have had the same problem when the bit moves from feed plane to retract it is a rapid movement and would miss steps. now to see if your are missing steps zero off the top and run your program and if there deeper the bring the bit back down to the top and look at your dro for z if you not at 0000 are very close your missing steps engraving has lots of rapid movements

[A000612]

I am very new to working with a CNC and acquired a homemade system from an associate to work with and learn. I usually do 2D stuff on it and find it fun but thought I'd try my hand at engraving. The problem is that the depth of the cut seems to change, it gets deeper, with every letter I engrave. I'm using Mastercam X3 for the engraving and Mach3 from Artsoft to run my machine.
The engraving is pretty simple so I didn't expect any issues. I chose "contour" for the toolpath and "window" then selected the text.
I've done many 2D things before without this issue so wondering why it happens when I'm engraving letters.
Any help is appreciated. If needed I can attach G code also
Image attached showing what the engraving did. I stopped it mid cycle since it obviously was having issues.

Just for S&Gs, try changing the font type to MasterCam's default (MCX Box Font) and running again. I engrave .500 MDF as well as alum stock. I have experienced issues when trying to use more 'elegant' fonts. Not to mention, wouldn't it be nice if the problem resided in the software and not the hardware?!

[hub]

Also try to over-ride the rapids (G0), (in the control) to a low value to see if it works better.

[bushwakka]

I also once accidentally rotated my text in the XZ or YZ plane, so the cam program actually made the text get deeper left to right. I had to start the design again to get rid of the rotation.


Sent from my iPad using Tapatalk

[Superman]

Please read his NC file

His maximum programmed depth is Z-0.008
- there is no issue with what he has created ( or output ) from Mastercam

It is a machine issue