From Manual to CNC - Sherlines

[zeeprogrammer]

You're using a Gecko G540? Did you insert the correct resistor for the current control? If not see the manual for value and placement.

I did insert a resistor. As for whether it is correct...I used 3.3K ohm which should limit amperage to just under the 3.5A max.
If it helps any, there's no load on the motors. Just a plastic flag to see it turn.

[Jasonb]

Zee just so you can see what it is like this is a simple turned part processed in F360. Basic piece of 12mm dia stock faced, spigot rough turned, spigot finish turned and then parted off to length.

You can see the various operations listed down the left side that get highlighted blue when they are taking place. Purple on the simulated part is waste material and green the finished surface. I just set cuts to 0.5mm (20thou) and a 0.25mm (10thou) finish pass. Part has 1mm of waste allowed for on t heend so it takes two passes to face that back to finished surface and so on.

<a href="https://www.youtube.com/watch?v=Ke7jnZUQRoU" target="_blank">http://www.youtube.com/watch?v=Ke7jnZUQRoU</a>

[Roger B]

Zee's spigot, the mind boggles 

[Hugh Currin]

Jason:

Thanks and you're right, the speeds I mentioned should be 7.0 in/min. Original post corrected.

The example does use a drilling cycle for the four small holes. However, it seems to use the 1/8" endmill for drilling. I guess it is just an example.

The step over in that example (from the CB model) is 0.4 (40%). I suspect this is the CB default.

I hadn't considered it but I like your scheme using depth first. It does use more of the side of the tool so tools should last longer. I'll try this next time I cut a pocket. Thanks.

Thanks.

Zee's example is running at 7" (180mm/min) not 0.7".

I've just drawn out the part and then used Fusion to do the CAM, not all the details are in the CamBam example as it does not mention speed and only gives depth of cuts (vertical) but no step over so I used approx 2/3rds cutter dia for stepover (0.080") and my max spindle speed of 5000rpm otherwise all as per the example. and it takes 30mins to run.

As said it's not how I would cut it, preferring to use more of the side of the tool and a 1/8" cutter would need long flutes to get through the 1/2" material, also don't fancy trying to get the swarf out of the hole when using it to drill the 3.6mm holes at full depth. Will run the CAM again with some settings that I would use and see what it comes out like.

[awake]

[I did insert a resistor. As for whether it is correct...I used 3.3K ohm which should limit amperage to just under the 3.5A max.
If it helps any, there's no load on the motors. Just a plastic flag to see it turn.

Is the 3.5A max the rating of the stepper motors? Or of the driver?

The more amps you are running through the motors, the hotter they will get. If you don't need as much torque, you can turn down the amps. Of course, you should not run the motors with more amps than they are rated for.

[zeeprogrammer]

Thanks Jason. Is that video of F360? How was the g-code generated?

Thanks Hugh. I also found a post-processor setting to use. I suspect I created the example using the default post-processor. I probably should have selected the Mach3 post-processor. I also see a Mach3-Turn post-processor. Not that I know yet what this does.

Is the 3.5A max the rating of the stepper motors? Or of the driver?

Of course, you should not run the motors with more amps than they are rated for.

I have the motors wired in parallel configuration. The current/phase in that configuration is 4.2A.
The Gecko drive provides a maximum 3.5A (but there's some question if that's really true. i.e. RMS or not).

My poor understanding is that the driver will only provide the maximum set by the resistor (i.e. 3.3A) and the fact the motors can take more shouldn't matter.

I chose this motor based on what I've seen other people do but it's been a question whether to wire in series or parallel.
Parallel has twice the current/phase but serial has four times the inductance/phase.
I don't recall now but I think it was the inductance limit that had me choose parallel.

Jason...the first part I hope to make (once I convert the lathe to CNC) is a bowling pin. Attached is an STL for imperial and one for metric. I use imperial.
However, these STLs were intended for my 3D printer and were drawn in the XY plane.
I suspect I need to rotate this or redraw using the XZ plane. No?
I believe that once I import a DXF into CamBam I have to delete everything except the profile line (i.e. 1/2 of the outline).

A fellow on the CamBam forum helped me out in finding the 'lathe-test.cb' file.
I felt really silly as it was in the ProgramData folder which I didn't even know existed (after all these years!!).
Also found it using the 'Tools' tab in CamBam and selecting 'Browse System Folder'. Not that intuitive for me.

[jadge]

The steppers on my CNC mill (Tormach) get hot after a long run, but not so hot you can't hold your hand on them. So probably around 60°C.

Andrew

[Mike R]

Zee
You can definitely turn down the amperage, 3.2A at 48V ~ 150 watts - so yes they will get hot.  Remember incandescent bulbs and how hot they got? 
You don't need 150 watts of power to drive the X or Z axis.  I think thats 2 times your spindle power?
As for post processors - it can have a big effect.  The way that arcs (i.e. G2 or G3 commands) are interpreted and / or commanded can vary and if done wrong on the lathe you'll end up with odd loops in space.  I can't help on CamBam or Mach3 as I don't use either (Fusion360 and LinuxCNC for me)

[Jasonb]

Yes that was F360 in all the video's. Did not produce the G-code but assume it is the same for milling where I just click the post processor button, though not sure if it actually has Mach3 Turn at least in the unpaid version just Mach3 Mill.

In Fusion it does not really matter what way the part is drawn as in the initial setup you can move the 3 axis about to suit the way the work wants to be machined eg if milling two sides of a part like the curved aluminium one s I posted last week in the dark side thread then I moved the axis for the second curve as the work was moved in the vice. It also lets you work on the 3D image rather than having to use a profile drawn as a DXF as you can see in my last video

Can you post those files as .STP Step files as I'm having a job picking up the axis of the STL files, also check your units as the metric one is about 2ft long.

[zeeprogrammer]

Thanks Andrew.

Thanks Mike. Right, that's 2x spindle power. Yes, I've come across references about the G2/G3 commands and loops.

Thanks Jason. I do not see any option for creating an STP file.
I don't know what's happening with the metric file. It loads fine in Cura and looks okay in Cubify Design. Should be 63.5mm (2.5") long.
I'm wondering if the file contains any unit information. If I load the imperial version into Cura, I get an object just 2.5mm high.

[kvom]

Gcode loops are caused by a mismatch in arc center mode between the CAM and the control.  For a G2 or G3 command, the IJK options state where the center of the arc to follow is located.  I highly recommend you use incremental, meaning the I and J words state the distance in X and Y to the center from the current position.  This is the default setting in Cambam.

https://www.cnccookbook.com/cnc-g-code-arc-circle-g02-g03/

[Dave Otto]

Gcode loops are caused by a mismatch in arc center mode between the CAM and the control.  For a G2 or G3 command, the IJK options state where the center of the arc to follow is located.  I highly recommend you use incremental, meaning the I and J words state the distance in X and Y to the center from the current position.  This is the default setting in Cambam.

https://www.cnccookbook.com/cnc-g-code-arc-circle-g02-g03/

Crop Circles, I used to struggle with them years ago when I first converted my mill; mostly due to using cutter comp at the control. When I quit using cutter comp and let the CAM software deal with it, the problem pretty much went away. When hand coding it is easier to let the control do the cutter comp as you have one thing less to think about. But with the modern CAM systems I'm not sure why anyone would want to do that anymore.

Dave

[zeeprogrammer]

Progress of sorts.

Found a video that showed a simple CamBam part (like a spigot!) with roughing cuts followed by finishing cuts.
Managed to create a g-code file.
Loaded that into Mach3 and was quickly confused. Didn't look right when I ran in simulation mode. In fact, it looked more like it thought the part was in a mill.

When I had installed Mach3, I had created both a mill and a lathe profile. It doesn't look like the lathe profile was setup right (or something).

Instead, I took the Mach3Turn profile that came with the app, configured the port and pins, and found myself looking at the part I wanted. 

So I ran it.

<a href="https://www.youtube.com/watch?v=BALlxbWVDFA" target="_blank">http://www.youtube.com/watch?v=BALlxbWVDFA</a>

So far everything looks as expected but you can tell something is wrong. The part is nearly 2" long but the Z axis motor only rotates maybe once as it traverses.
Somewhere there should be a setting for configuring the gear ratio etc that says the motor has to turn so far to move a given distance.

I also recall something about handling backlash and various offsets that I need to look into.

I will admit, I'm still vacillating between giving this up (it's way more work/learning than I had counted on) and plowing on.
I'll plow on some more.

A little  goes a long way.

[Elam Works]

But with the modern CAM systems I'm not sure why anyone would want to do that [use cutter comp] anymore.

Using cutter comp makes it easy to make corrections for the finished size, without re-posting the program. However I'll admit I do not use cutter comp for roughing passes. I rely on the correct tool radius and the roughing allowance in the CAM software. Its close enough for roughing.

That is for 2D and 2-1/2D. For 3D my CAM package will post for cutter comp, but the CNC mill cannot deal with it in its tool offsets. So I rely on defining the tool nose radius in the CAM package and posting 'without comp'. Generally when doing full synchronous 3D, the results are close enough because typically it is a sculpted surface replicating a casting or forging (a forgery!), that short of a CMM, I cannot inspect anyway. It has to visually look right more so than meet a particular tolerance. But if it did include a feature of size that I could measure with normal workshop measuring instruments, then I would have to define the tool in the CAM package as larger or smaller radius than it really was to get the desired feature size. Usually those features can be split out and done with other tools using cutter comp.

-Doug

[kvom]

Cambam doesn't generate cutter comp in g-code.  I've used it for dialing in threadmills but needed to edit the code to add the G4x codes.

As for the z axis motor, it needs to be configured to match a hypothetical leadscrew.