From Manual to CNC - Sherlines

[crueby]

For videos I usually upload to youtube, and post the link from there.

[zeeprogrammer]

Now to take apart the franken-system and move things over to the machine bench.

Oops. Getting ahead of myself. Before I take it apart and move it, I'll create and run a lathe and/or mill g-code program and cut some air.

[crueby]

Now to take apart the franken-system and move things over to the machine bench.

Oops. Getting ahead of myself. Before I take it apart and move it, I'll create and run a lathe and/or mill g-code program and cut some air.

Make sure you anneal the air so it cuts easier!

[zeeprogrammer]

Now to take apart the franken-system and move things over to the machine bench.

Oops. Getting ahead of myself. Before I take it apart and move it, I'll create and run a lathe and/or mill g-code program and cut some air.

Make sure you anneal the air so it cuts easier!

It's my shop. The air is always annealed. 
Either by words or deeds.

[zeeprogrammer]

Not being able to use my left thumb, I've put my finger treadle project on hold and now learning more about CamBam and Mach3.

One area I've always had trouble with is 'speeds and feeds' or 'cutting speed and feedrate'.

I think I've got a handle on cutting speed where the idea is to determine spindle speed.
I know there's several ways to calculate or estimate RPM. Here's one...

RPM = (SFM / diameter) * 3.82 * correction factor

SFM (surface feet per minute) seems to be a value taken from a chart of materials.
diameter is the diameter of the workpiece (lathe) or tool (mill).
3.82 is a constant (some people use 4, others use pi).
The correction factor seems to depend on tool type (HSS or carbide). For example if carbide is used then the factor is 2.

Finding said chart has been difficult and I'm not sure there's agreement across the board.
It seems to depend on material type, material hardness, mill or lathe, tool type, drilling or not, etc.

Question...what do you people use to determine spindle speed?
I'm not doing production nor looking to be a 'professional'. I'm looking for rules-of-thumb.

I'm having more difficulty with feed rate which seems to be a function of the number of flutes and depth of cut (or size of chip).
Question...what do you people use to determine feed rate?

This all sounds fundamental and even though I've been at this hobby for some 10 years...I've been winging it.

Having played with the machines for a little bit, I've decided to convert the lathe first. I may end up not converting the mill (or at least waiting until I have a project where it would be an advantage).

Thanks

[Jasonb]

I've mostly been using the tool library that comes with F360 as a basis for speeds and making small adjustments mostly reduction in feeds. I also look up the charts from the tool makers who give speeds and feeds for various materials and type of cut/cutters.

[mikemill]

Zee

Charts and graphs are all well and good but there is nothing better than experience
I you look at you tube video's of CNC mills the tool is running at 10k rpm and the feeds are whizzing around, don’t try to emulate.

Basic principles say for a 1/4in dia end mill, ere on the cautious side to start with
For steel speed 1k to 1.5k rpm feed 2-3 in per min plus suds
      Brass speed 2k to 3k rpm same feed to start with
      Aluminium same as brass but needs suds as ali is very sticky
There are special cutters for ali with wide gaps between flutes to avoid sticking
Just go slowly and be VERY aware of G0 rapid movement, its faster than you can get to the E stop.
Good luck and enjoy CNC when you get used to the process it is very rewarding.

Mike

[Jasonb]

Zee, if you watch any of my videos in the "over to the dark side" thread on youtube I usually put the cutter, speeds, feeds, cut etc in the description so that may give you an idea of what works on my machine.

Typically for a 6mm cutter on steel I would be 2.5-3K rpm feeding at 200-400mm/min Aluminium would be at my max 5000rpm.

[kvom]

I can recommend that you buy G-Wizard for f&s.  I have recouped its cost many times over in tools that I didn't break and work not gouged.

cnccookbook.com

[kuhncw]

I've found G Wizard very helpful as well.  The program lets you vary feeds and speeds to minimize cutter bending

Chuck

[jadge]

I've tried a few F&S calculators and didn't get on with them. I'd rather compute my own numbers based on experience and manufacturer data. The two important parameters are spindle speed and chip load (which determines feedrate).

For spindle speed as a starting point I use the figures in Machinery's Handbook. I might downgrade them a bit especially for tougher materials like stainless steel. I simply divide the wanted cutting rate (feet/min) by the circumference of the cutter (diameter x pi) to get a spindle speed. For smaller cutters (<6mm) my CNC mill is often the limiting factor.

I take chip load (in thous) values from manufacturer datasheets, plus experience of what worked. Feedrate is chip load times number of flutes times spindle speed. The chip load varies with the type of cut. A full width and one diameter deep cut will be at a lower chip load than a full depth, but shallow width cut. Read up on chip thinning.

For finishing I usually climb mill but for roughing I use both, otherwise the cutter spends ages lifting and traversing to the beginning of the cut rather than just going back and forth and cutting in both directions.

Of course one needs to take into account the size and rigidity of the mill. I learnt that it's better to use smaller cutters running at high spindle speeds and feedrates rather than larger cutters running more slowly as one might do on a manual machine. I rarely use cutters bigger than 10mm on my CNC mill.

I use YG cutters (Korean) and their speed and feed tables seem pretty reasonable. Certainly not the all out industrial stuff you see on youtube. The biggest problem is that for cutters smaller than a few millimetres my mill runs out of spindle speed.

There are two important points to note. Do not feed too slowly, the cutter needs to cut, anything else just rubs the cutter and destroys the edge. This is just as important on a hobby CNC mill as an industrial mill. The metal and cutter do not know what sort of mill they are on. Second get rid of the swarf either by flood coolant or airblast. Nothing fudges a cutter quicker than recutting swarf.

I normally do a roughing pass and a small width of cut finish pass to get the best finish.

Andrew

[zeeprogrammer]

The problem with 'experience' is that I virtually don't have any and what machining I've done is without knowing what feed rate or speed I was using. I mainly did what sounded and looked okay.
Experience equates to months, if not years, of learning so I can't depend on that yet.

Going through various documents and videos has been frustrating. Too often I come across statements like "and calculate X using the desired Y" but I have no idea what Y is.

I'm looking at the setup screen for G-Wizard.
I found the min/max spindle speed for the lathe.
Spindle Power was an issue. I came across 70 watt for the Sherline which I believe is 60/745.7 = .08 horsepower. No?
Now I'm stuck again on 'max feedrate'. No idea and can't find anything other than one statement that seem to indicate something around 18 ipm.

I'm a procedural kind of guy and this stuff is exceedingly frustrating.

As for the Machinery Handbook. $72 and I don't know what it provides. Some charts for speeds/feeds? Is that the only source? What else does the book provide for the hobbyist?

[awake]

Zee, I find Machinery's Handbook useful from time to time ... and sometimes interesting just to read through bits of it. But I wouldn't spend $72 on it. I bought a copy well-used for a few bucks many years ago, but since then I've discovered that there are some .pdf scans of older editions on the internet. Not sure how legit they are, but I think - ?? - there may be a Google Books version, which I would presume to be legal.

[zeeprogrammer]

I have to admit I'm really in the dumps.

[kvom]

The only pages in Machinery Handbook I have used many times are those with the specs on threads when I wanted to single point.  On occasion I might look up something new, but I haven't opened my copy in a long while.

Max feedrate is whatever your rapids are set to.

The Sherline DC motor is .06W at 6100 RPM, but is higher at lower RPM.  It replaced a 1/2 HP motor according to Sherline.