From Manual to CNC - Sherlines

[fumopuc]

Hi Zee, Jason, if this is the chosen spindle speed, it seems to me more than slow.


May be this link on how to calculate for hobby purposes will help.
https://webseite.sorotec.de/download/fraesparameter/schnittwerte_en.pdf


If you cannot archive the in the first calculation recommended spindle speed, than it can be reduced to what is achievable in the second part of the calculation.
I prefer not to overload a cutter.
That means Ap, depth of the cutter into the material 1/5 of cutter diameter in aluminium and 1/10 of cutter into steel.
By milling a slot, that means 1/2 diameter of the cutter and the ground are cutting material , it is better to use even less.
 
Ae, width of cut (from the side), 1/3 of cutter diameter.


May be this will help you over all to find your way of CNC machining.

[Jasonb]

That's one reason I asked the size of the part 972rpm would be OK for certain diameters and if it is large then cutting times will be longer than a small dia part.

Though feed per rev would work out at 0.025" ( 2" /972) which is quite aggressive for a small machine even  0.05" DOC.

Zee if you can post the part file I'd be interested to see what it comes up like in F360 if I base it on the type of cuts I could take with my Unimat. Either the Alibre part file or .STP would do.

[jadge]

Hmmm, 2"/min feed and 972rpm spindle speed is 2.06 thou per rev. Seems pretty low to me, but I run a bigger lathe.

Andrew

[zeeprogrammer]

Thanks guys.

The part was created from an example CamBam, found here...

http://www.cambam.info/doc/plus/SimpleExample.htm

The size is 5" x 2.375" and 1/2" thick.
All the settings were given in the example. Such as 7 ipm feedrate, 2 ipm plunge rate. Tool diameter is 1/8".
There is no spindle control.

All I did was load the g-code file into Mach3 and ran it. I hadn't set/changed any settings in Mach3 (thinking the program does what's needed).
I haven't read the g-code to see what it does.

Attached is, what I think is, the drawing file from CamBam.

I loaded the g-code in the Mach3 simulator and it gave a 59 minute run-time.
The example may not be real-world but was good enough to make some progress.

I'm still curious why the motors got too hot to touch. However, I haven't done any motor tuning or checked what controls there are for setting acceleration etc., or what, if anything, I should do to optimize.
I know there's a procedure for tuning the Gecko drive which I haven't done yet.

[kvom]

Don't use the 0.9.8 CB files,  1.0 is the official release now.

[zeeprogrammer]

Don't use the 0.9.8 CB files,  1.0 is the official release now.

Is there a particular reason or just because it's newer? (1.0 was released end of February but I don't know the year.)

I tried tuning the Gecko driver. The procedure is to run the motor at 2 rev/sec and adjust a trim pot until an audible sweet spot is heard.
I couldn't figure out how to run the motor at 2 rev/sec so I just held the jog button down. I could hear a slight difference as I trimmed the pot but I can't say I detected a 'sweet spot'.
Of course, having lost the ability to hear higher frequencies may be part of the problem.

Lots to learn...
1) If I run a CamBam generated g-code file, what settings on Mach3 need to be addressed?
2) What motor characteristics (if any) need to be set and where? (e.g. maximum acceleration).

I'm still hoping for any thoughts as to why the motor got too hot to touch. Driving too fast? Driving too long? Something else?

[Jasonb]

I thought you were running something for the lathe, that looks to be a part milled out of plate

[Hugh Currin]

Zee:

I'd also start by CNCing the mill. It will be more useful and there are far more examples and help available for milling than turning.

If I'm seeing it correctly the example cuts a 1.5" diam pocket 0.064" deep then a 0.5" diam pocket 0.51" deep. I think a 1/8" end mill is small for this part and may be one reason it runs so long. Try to run it again with a 1/4" end mill, which is what I'd use in the Sherline (probably 3/8" in a larger machine). CamBam used 10,000 rpm spindle and 7.0 in/min feed rate, Little Machine Shop calculator suggests 6000 rpm at 7.0 in/min (if 2 flute/HSS end mill in aluminum) so 7.0 seems reasonable. Also, increase the depth of cut from 0.02" to 0.022" for the first pocket. That reduces the number of passes from 4 to 3 (unless you want that last 0.004" pass for finishing.

I understand that stepper motors run hot. Those on my Sherline are too hot to comfortably touch. 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.

Good progress.

P.S. And as Jason says, it is a program for the mill. :-)

EDIT: Speeds should be 7.0 rather than 0.7. Changed in text.

Thanks guys.

The part was created from an example CamBam, found here...

http://www.cambam.info/doc/plus/SimpleExample.htm

The size is 5" x 2.375" and 1/2" thick.
.................
I'm still curious why the motors got too hot to touch. However, I haven't done any motor tuning or checked what controls there are for setting acceleration etc., or what, if anything, I should do to optimize.
I know there's a procedure for tuning the Gecko drive which I haven't done yet.

[jadge]

CamBam used 10,000 rpm spindle and 0.7 in/min feed rate, Little Machine Shop calculator suggests 6000 rpm at 0.7 in/min (if 2 flute/HSS end mill in aluminum) so 0.7 seems reasaonable. Also, increase the depth of cut from 0.02" to 0.022" for the first pocket.

Wow, those are slooooow feeds, and are why I prefer to do my own calculations. The pockets on these steel parts were done with a 3mm cutter:



I was running at 5000rpm and 120mm/min (4.7"/min). I was using a 3-flute end mill but even so 0.7"/min is incredibly slow. For pocketing I was cutting with a width of cut of 75% of tool diameter and 24 thou depth of cut. I left 8 thou for a profile pass which was done at 0.093" depth of cut, ie, 3/32". Machining time for the two pockets in the part on the left was 16 minutes.

Andrew

[Jasonb]

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.

<a href="https://www.youtube.com/watch?v=6VbaBdNF9k8" target="_blank">http://www.youtube.com/watch?v=6VbaBdNF9k8</a>

[zeeprogrammer]

I thought you were running something for the lathe, that looks to be a part milled out of plate

Sorry about that but yes. I didn't find a CamBam example for the lathe so I used a mill example.
Remember though, I'm not running on an actual lathe or mill. I'm running a frankensystem that just has two motors turning air.
No doubt that means certain parameters are not optimal but the point was just to run Mach3 and a couple of motors.

Currently trying to create a part in CamBam for the lathe but it looks like I'm missing something. Perhaps a lathe plug-in.
I'll try downloading version 1.0.

...just saw a couple of posts...

The project I have in mind (the spinning wheel) doesn't have any parts (so far) where a CNC mill would be an advantage. All the mill parts are easily done manually.
However there are a couple of parts (legs and finials) that having interesting curves making manual machining extremely difficult.
Given the availability of help with CNC Mill, I can see where it would be easier in learning CamBam and Mach3 but I'm not sure it really reduces the learning curve for the lathe.

Remember...I'm learning on a frankensystem where I only have two motors (i.e. a lathe). No spindle, no tool, no anything else. I could easily add a third motor.

P.S. Max spindle speed is 2800 rpm. Sherline offers a pulley accessory that provides 10000 rpm (which I don't have).

Just saw Jason's post. That seems to indicate the example I used from CamBam is not real world (but was good enough to learn something).

[Jasonb]

Just as an example Zee I redid the plate as I would probably cut it using a 6mm cutter and then swapping to a brill bit for the tapping holes. Also used full depth for the pocket and a tame 0.040" stepover and 12ipm feed.. Same cutter for the 1/2" hole ramping down at 2degrees in two passes so only half dia of cutter being used. Peck drilling to clear swarf and it came out at 8mins, even allowing for your slower speed spindle that would come out at abbout 15mins.

<a href="https://www.youtube.com/watch?v=8jqjm3J8ef8" target="_blank">http://www.youtube.com/watch?v=8jqjm3J8ef8</a>

I did try the F360 lathe option this morning for the first time and it was quite easy to face a part, rough turn a spigot and then do a finish pass, you could have a go at that to get some idea of the G-code. If you can attach a stp file of the turned column I'll see what it comes out like.

[zeeprogrammer]

Thanks Jason. That's interesting and shows there's ever more to learn. Stepover? Choice for 12 ipm feedrate?

What application are you using in the video (I can't read it)?

I'll need to redraw the column and will get back to you.

In the meantime, I downloaded CamBam 1.0 but I didn't see any real change in folders and contents.

I'm looking for 'lathe-test.cb' which according to CamBam is in the 'Samples' folder. But I can't find any 'Samples' folder nor a source for the file.

[Jasonb]

Stepover is how far the tool moves sideways each time it goes round that 1/16" deep pocket, I set it at 1mm which is quite a light load and should be the sort of thing your mill can handle eg 0.050" deep x 0.040" horizontal. I would be using nearer to 4mm on my machine and that would still be quite light.

Feed is again light considering the depth and stepover but better to be safe to start with. assuming a 3 flute cutter this would be about 1/3rd of the book feed rate giving a chip load of 0.02mm per tooth rather than 0.06mm.

I drew the part in Alibre as that is what I'm used to and then exported it out as a .stp file which I then opened in Fusion 360 and used that to do the CAM and create the simulation

Yes there are so many variables that can be tweaked to get the best results both in time, tool life and finish and I've only scratched the surface. If you are using mill code then you may be better off with the X&Y motors running as they are the ones that move the most.

[zeeprogrammer]

Thanks Jason.

If you are using mill code then you may be better off with the X&Y motors running as they are the ones that move the most.

Good point.

I just registered on the CamBam forum. Odd that I only found 4 references to 'lathe-test.cb' but little else. Looks like a bunch of helpful people though.