[nlh205]

Hi, I have a desktop cnc that I have built myself and have started using. I have been trying different cam software and really like CamBam. But I am having trouble with the precision of CamBam. I cut a 1"x1" square through CamBam using 0.125" endmill and finished product is smaller by 0.020". When i run the same .dxf file through MeshCam and cut it with the same endmill i get a result within +-0.005. I have milled many different pieces for testing and CamBam is always smaller. Also I am using Sketchup for cad and mach3 for posting for both CamBam and MeshCam. Any help would be appreciated.

Note: I hope I have posted this in the right forum, if not I am sorry. Thank You.

[ger21]

Are both cuts in the same direction? Can you post the .dxf file and the g-code from CamBam.

My guess is your seeing deflection when running the code from CamBam.

[nlh205]

Thanks for the response. I have the dxf file below and will post the gcode because i could not attach the .nc file.

( Made using CamBam - http://www.cambam.co.uk )
( 1in-square 6/27/2014 7:55:11 PM )
( T0 : 0.125 )
G20 G90 G64 G40
G0 Z0.125
( T0 : 0.125 )
T0 M6
( Profile1 )
G17
M3 S1000
G0 X1.0625 Y0.0
G1 F6.0 Z-0.025
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.05
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.075
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.1
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.125
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.15
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.175
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.2
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.225
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.25
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.275
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G1 F6.0 Z-0.28
G1 F14.0 Y1.0
G3 X1.0 Y1.0625 I-0.0625 J0.0
G1 X0.0
G3 X-0.0625 Y1.0 I0.0 J-0.0625
G1 Y0.0
G3 X0.0 Y-0.0625 I0.0625 J0.0
G1 X1.0
G3 X1.0625 Y0.0 I0.0 J0.0625
G0 Z0.125
M5
M30

[ger21]

The g-code from CamBam is correct. I suspect that the bit is being pulled into the material, resulting in a slightly smaller cut. If you cut in the opposite direction, you'll either see a correctly sized part, or a slightly larger part.

Can you post the MeshCAM code? Change the extension from .nc to .txt, and you can upload it.

[nlh205]

Here is the meshcam file.

[nlh205]

I think you may have found my problem. I changed the milling direction in cambam from conventional to climb and now I am get the same results as meshcam.

[ger21]

The "problem" is a lack of rigidity in your machine.

[nlh205]

Could you please explain? If it was a lack of rigidity in the machine. Why would a change in direction change the outcome and why would i get constant results in the same range on different cuts?

[Trotline]

The direction of cut determines whether you're "climb" cutting, vs "conventional" cutting. Climb cutting tends to impart a force on the endmill that's directed away from the part, while conventional tends to pull it towards the part. There's some small amount of give in the material, but a lot of the difference you're seeing is caused by flex in the machine's structure. It's an illustration of why most builders spend a lot of time and effort to maximize rigidity, and why few routers can do a good job milling aluminum, where the forces are greatly magnified.

Very high rigidity is out of reach for most homebuilders, and it's something you can work around, so it's not a cause for major alarm. Mostly, just pay attention to your cutting direction for repeatability, and start analyzing the machine to see if there are weaknesses that you can address. It's all part of the hobby.

Luke

[nlh205]

Thanks for the explanation. I am new to cnc machines and I have a lot of interest in them, so I made one myself. I never really thought that the direction of cutting would change the end result but after the explanation I understand. So thats why when changed my CamBam direction to climb I got the same results as MeshCam. So what method of cutting would be considered normal: Conventional or Climb? Also how would I check my machine for rigidity, would that be my off distance from the conventional cutting direction?

[ger21]

In most wood and wood products, conventional cutting will give a cleaner cut. One thing you can do is a "roughing" cut about .02" oversize, then follow with a finishing cut. The lighter finishing cut won't be pulled into the material like a full cut will.

[nlh205]

Thanks ger21, that makes much more sense now. But I am hoping that i will be able to cut aluminum successfully at some point in time. The machine i have is a myDIYcnc. I have the plans and went by that. I have made some customizations to my liking and also to what i thought would give me extra strength and prolonged life. I have no clue what my rigidity will be but all my previous cuts were made with my spindle being attached by a few zip ties and tape. Lol. So i am cutting out some custom spindle mounts tonights and hopeful my cnc will perform to a better degree. Do you think that this cnc will be able to cut aluminum successfully with proper strength and also any tips on cutting aluminum for the first time? Thanks.

[Trotline]

Pictures would be helpful in answering that sort of question. Without knowing what modifications you made, all we can go by is the base machine. My guess is that aluminum would be more than that design can really handle, based partially on the unsupported rails, and partly on the spindle, Overall, the design isn't very beefy, and aluminum really requires beef. Supported rails are far more rigid than unsupported. You wouldn't think steel bars are flexible, but they really are, when a load is applied.

The way to measure the flex in the system is to put a dial indicator against the cutting tool, and then just push on it, to simulate the cutting forces. You'll then see what sort of flex, side to side, and back & forth, is present. From there, you try to deduce what components could be flexing and how to strengthen them.

Luke

[nlh205]

Thanks for the tips Luke. I'll keep them in mind before i trying cutting the aluminum. I will probably build a new gantry system with rollers instead of rails or a new machine of my own design. Only built that machine because it was my first one and it was small and easy to work with. Also thanks for the posts guys it have really helped.

Nate

[ger21]

For aluminum, always climb cut

[atwooddon]

If you have the earlier machine (before Bigfoot) you will probably have trouble machining aluminum. The machine was not designed to do that, ie gantry uprights, rails, table, spindle, are just not up to the task. You might be able to take very thin cuts repeatedly to accomplish the machining but it will be slow. Not being critical of the machine, but it is just not designed for that task. I have followed the development of these machines from inception and it does offer an easy way for someone to get started but you have to recognize the limits. Another consideration in accuracy is the spindle. The typical Dremel like tool is just not intended for this kind of use and will develop excessive runout quickly. Additionally, the chuck holding the bits can create additional runout issues affecting accuracy. Like I said, not trying to criticize the machine, design or the company, they provide an easy way to get started but this machine (actually every machine) has limits you have to work within.

My first machine was just terrible yet was a great tool for learning about software, techniques, tools, and what 'not to do'. Actually, I learned a bunch about what 'not to do'.... ;-)

Don