Lessons learned and Work Flow check list

Mostly Printed CNC - MPCNC Advice
1

All,

(I’m not quite sure this is the correct category for this post, but please move it if it isn’t.)

Sorry for the long post, but I wanted to capture everything while it was fresh in my mind.

I finally got to cut my first real project, an Instrument panel.

In the process I dealt with a couple software issues (EstlCAM), mechanical stupidity, and getting the steps just right (which saved my butt when part of the cut failed).

Mechanical first: I’m using the Dewalt 660 and I while I saw something about using the builtin “wrench” to tighten the collet, I found that it is pretty worthless! I almost lost the whole part when the collet was too loose and the bit came out part-way through the cut. The bit is an upcut and it just walked itself down into the wasteboard, gouging the hole out of round. Fortunately I was able to get the bit reinstalled and because I had documented the setup I was able to restart the cut without any additional mechanical problems. Lesson learned: USE A REAL WRENCH TO TIGHTEN THE COLLET NUT!! It’s just really tough to get it tight enough with the nose piece wrench (which will be removed the next time I take the router off the mount).

EstlCAM challenges: The first few cut attempts looked like an extreme slow-motion video. The head moved quickly to the location and then just seemed to make barely perceptible motions while making the hole. I went back over the settings in the EstlCAM Basics and one of the settings was not shown in the same way in the current documentation as the software shows it: Z-Plunge ramp angle. I had it set to 1 degrees, which is WAY too shallow. I reset it to 45 degrees and that seems to work fine. I suspect I can set it to 90 degrees and still cut just fine in my materials. Also Plunge depth and cut-depth have some funny interactions if they are not coordinated. I don’t yet have a complete understanding of how that works, but for the moment I can cut. Another EstlCAM foible is that when you first load a DXF file, it wants to place the tool path origin at the lower left point that is the extent of the drawing elements. I wanted my tool path origin to be in another location, further left and down (due to the way my non-flat part needed to be cut). I did this by adding a small circle on the drawing where I wanted the tool origin to be. I could then select that point in EstlCAM for the origin point.

Lastly, my setup, documentation, and work flow checklist. Two terms that I think make some of the explanation easier to understand: Machine origin is the location the core moves when I ask it to home (square) the trucks. Work origin is the location on the workspace that I want to use as the 0,0 point for the cutting. I mounted a smaller wasteboard for this project that I expect to reuse when (if) I do another panel for this glider type. I squared it to the table and homed the trucks, then moved the PEN to the point on the wasteboard where I wanted to start the cut (workspace origin). An important point here, this point will be the same as is shown in EstlCAM for the origin of the tool path. It is the one I selected using my added circle on my drawing. I then noted the machine coordinates (X,Y) for that point relative to the homing position. Now I can get back to it even if I turn the machine off. Using the pen I drew X and Y lines to help me verify that location in the future. I also made other notes for lines I needed to orient the part, but that is not part of the general work flow.

To start a cut I do the following at the MPCNC:

  1. Move the core close to the machine origin (I need to get my machine size correct in the firmware as it does a reset if I try to home for too far away). You may not need to do this step.

  2. Power up the machine and home the axis using the V1 Menu (I have a TFT display and am still using sneaker-net to move files to the machine).

  3. Use the motion control to move the X and Y to the work origin point, using the values I determined when drawing the reference point.

  4. Move the Z axis to the work surface, either with the homing plate (using the V1 menu) or manually.

  5. Reset all coordinate values using the V1 Menu.

  6. Load and “print” the gcode file on the SD card.

These steps allowed me to save the cut when the bit fell out of the collet. I was so glad I had done all the documenting of the location values. It made it easy to restart with the confidence that the tool wasn’t heading off to the wrong location(s). I only had one blank part to use for this cut, there wasn’t a second chance without a LOT of rework or re-manufacturing.

I’m sure some of the steps will be modified when (if) I start using Repetier-host or some other program instead of the TFT screen. For the moment I’m just happy I have a working process and checklist.

I hope this helps someone else, and thanks for listening!

Mike

4 Likes
2

I’m not sure what version of the firmware you are running. In the latest version (510), the default table size in the firmware was increased to 600mm, so this is not as much of an issue as the 200mm it was before. Personally, I think this number should be increased to 2000 so that it never gets in the way or require an edit of the firmware. If you decide to edit the firmware to set the size to your work area, it is these two defines in configuration.h:

// The size of the print bed
#define X_BED_SIZE 600
#define Y_BED_SIZE 600

USE A REAL WRENCH TO TIGHTEN THE COLLET NUT!

I found this out fairly quickly. I also found that when I used the built -in tightener, I was putting enough pressure on things that I sometimes managed to move the router even though the steppers were still engaged losing my home position.

Reset all coordinate values using the V1 Menu.

In EstlCam (Setup/CNC Programs/Texts/Program Start) you can add a G92 X0 Y0 Z0 to be automatically inserted at the beginning of your g-code file. This will eliminate the need to use the V1 menu to reset the coordinates.

2 Likes
3

just make sure your bit is really at z0 if you do this.

Silly me forgot I had this in my gcode the other day. I had moved the Z axis up a few mm to take a look at something. When I hit ‘go’ it reset that to z0 and then air-cut until I realized I had goofed.

4

Mike,

I don’t know if this helps at all but you can set your work origin in ESTLCam with the “Zero” tool.

ESTLCam_Zero-1
ESTLCam_Zero-13840×2100 619 KB

ESTLCam_Zero-2
ESTLCam_Zero-23840×2100 500 KB

It will want to snap to the nearest point in your DXF if you get to close to the drawing, but this is relative to your zoom level so you can get closer, if you zoom in further.

5

Tim,

Yes I know about the reset origin, but you have to have something in your DXF to snap to. I wasn’t able to figure out any way to offset to a negative position in “free space” completely outside the DXF lines.

I just will put a small point in the DXF to provide to option to select a cutting origin wherever I want it to be.

Thanks for making sure I knew about the reset O.

Mike

6

Mike,

What I mean is that you can place the origin arbitrarily anywhere inside, or outside of the drawing. It will try to snap if you get to close to the line, but it doesn’t require a point to snap to, to be placed. But then again, I don’t see a way of doing this with a very fine degree of accuracy, if that’s what you mean.

7

Alternatively, if you know the XY coordinate of your part in relation to the 0,0 point of your machine, you could manually add the following lines:

G0 X<x offset> Y<y offset>
G92 X0 Y0

I think ESTLCam has an option to add custom code to the beginning of the file. You could put it there and it’ll add it. Just remember you did this, because it’ll add it to all files.

That should move the machine to the 0,0 point of your work surface and then reset 0.

8

David,

I can try this next time I do a cut.

For the moment I’m deep in the process of finishing the Instrument panel. I want it off my plate so I can not feel guilty if I go fly my own glider: Schleicher ASH-26E motorglider.

Mike