Hey guys - I understand that this has been covered to death probably but I did search and read a lot of threads but am still a little confused. I have been using my Shark for quite some time and haven't had too many issues but want to get things right going forward.
I have a Bosch 1617 router - variable speed from setting #1 - 8000rpm to setting #6 - 25000 rpm
Here is a break down
#1 - 8000 rpm
#2 - 11400 rpm
#3 - 14800 rpm
#4 - 18200 rpm
#5 - 21600 rpm
#6 - 25000 rpm
So I did find a chip load table on here that seems quite straight forward - The chip load chart has an example of a 3/8" bit working through hardwood with a value of 0.015" - 0.018" - this relates to a formula of Chip Load = Feed Rate (ipm) x (rpm x # of flutes) So for a 2 flute upcut ballnose bit and an 120 ipm the rpm should equal 14,500, which would be a setting of about just under #3 on my router.
Is this sound logic? I have been running my rpms quite a bit higher but this does seem reasonable, to me?
Also - this assumes that a constant speed of 120 ipm. I notice with my machine it slows quite a bit in corners and curves as apposed to straight line cuts. Is this related to the software? For instance Cut3d or Vcarve Pro? I have talked to others that use Mach3 or other controllers that do not have issues with the slow downs in feed rate. Any input is greatly appreciated. As I have said I have been using it quite a bit and may slow down my rpms as a result of the calculation above. I really like the WYSIWYG aspect of both Cut3d and VcarvePro but would consider another control software to augment my abilities if it makes sense to do so. I would also like some advice on that front. Thanks
Regards Peter.
sppeds and feeds - sorry
Moderators: al wolford, sbk, Bob, Kayvon
Re: sppeds and feeds - sorry
Feeds and speeds are a complicated issue that involve more than just chip loads. Assuming ideal materials, tools, and machines you would determine your max RPM then use that to figure out your feed rates.
RPM -Metal
For metal and some composites this is easy using a SFM (surface feet per minute) number.
RPM=(SFM * 3.82)/(cutter diameter in inches).
e.g. 3/8" cutter in 6061 aluminium, SFM 800 - (800*3.82)/0.375 = 8,149 RPM.
RPM -Wood
For woods and soft media determining RPM is harder as it is a more variable material and things like moisture content will change the required feeds and speeds. A good test is to run a quick cut in the material at various RPMs and listen to the cut. To test the feed you can use the following method.
Set a RPM on your router/spindle.
Use a known safe/low chip load number (2% in woods 4% in plastic).
Test Feed=(Diameter)*(safe chip load)*flutes*RPM
e.g. 1/4" 2 flute in wood at 11,400 RPM - 0.25*0.02*2*11400 = 114 IPM
All test cuts should be at 1 diameter deep per pass.
If the tool squeals than your RPM is too high. Try reducing RPM, recalculating for feed, and test again. Might need to switch to a smaller tool if you can't get the cut to not squeal at your lowest RPM.
In general tools 1/8" and smaller are not going to squeal at all at anything other than absurd RPMs (100k).
Feed
Now that we have a good know RPM we can calculate for feed. Be careful when looking at chip load numbers. I have seen them listed as both total and per flute depending on manufacturer.
Feed = (total chip load) * RPM.
e.g. 0.004 total chip load at 11,400 RPM - 0.004*11400=45 IPM
Real World
Now lets talk about the real world where we don't have perfect materials, machines, and tools. Deflection, runout, material variability, tool quality/geometry, etc will all effect the best feeds and speeds you can use. I'll run through the basics of a couple common factors.
Deflection
Deflection can be a huge limiting factor in proper feed/speed. Deflection is basically the tool or machine bending into the cut to due to the cutting forces. The weaker the components in the cnc the more machine deflection in the cut. This is why you see metal milling machines made out of cast iron with small work areas.
A quick test to see how much deflection you have is to make 2 cuts with a small gap between them. The cuts should be in alternating directions leaving a small gap where they would meet. Think of it as a straight line cut from each end toward the middle. If you have deflection then you will see that the edge of the cuts don't line up. They will be offset by the deflection. The larger the tool and the more aggressive the cut the higher the machine deflection will get.
Runout
Runout is how much eccentricity ("wobble") the tool has while rotating. Think of the bit rocking side to side as it rotates. This is usually due to poor collets or routers/spindles not having proper mating surfaces or bad bearings. The more runout in the system the worse your cut quality will get and will limit your feed. It can also limit the minimum size tool you can use and shorten the life of the bit. You may also notice that your tools are cutting larger than spec. This could be due to a poor tool but a perfect tool in a machine with runout will cut larger.
Material variability
Graded metals are usually pretty uniform. Plastics and woods are not and this means that even on the same machine your feed and speed may need to change.
For plastics things like the manufacturers mix, cast or extruded, or even temperature of the material can all change how the material machines.
Wood has a LOT of variables. Grain structure, moisture content, and silica integration are a few of the issues that come to mind.
End result
What this basically all comes down to is that while chip load numbers can be a good starting point they will usually not end up being the sole factor in getting the proper feeds and speeds. The best thing to do is take those numbers and run a test. This will get you what YOUR feed and speed should be for YOUR machine in YOUR material. We recommend running a "zigzag" test cut using your starting numbers with increases in feed at each "V". I would go into more detail on this but that's a whole other post (and this one is already quite long). A lot of this is covered in more detail on our site but I don't want to post link here as we sell bits. Another good resource for this is CNC cookbook (Link).
Acceleration
As to your question on the slow downs. This is the effect of acceleration and look ahead in the controller. Basically the software is looking at the upcoming curve and calculating how much it must slow down to keep the cut accurate. It does this because you don't want the machine to slam the tool around as fast as it can. That would be bad for the machine, bad for the tool, and give a poor cut. A good way to think of it is a car taking a sharp turn. You wouldn't want to take that turn as fast as your car could go. You slow down to take it safely and smoothly. This can obviously be changed although I don't know if you have access to this in the shark controller.
Hope that helps. If there is anything I can expand on or anything else I can help with please let me know.
RPM -Metal
For metal and some composites this is easy using a SFM (surface feet per minute) number.
RPM=(SFM * 3.82)/(cutter diameter in inches).
e.g. 3/8" cutter in 6061 aluminium, SFM 800 - (800*3.82)/0.375 = 8,149 RPM.
RPM -Wood
For woods and soft media determining RPM is harder as it is a more variable material and things like moisture content will change the required feeds and speeds. A good test is to run a quick cut in the material at various RPMs and listen to the cut. To test the feed you can use the following method.
Set a RPM on your router/spindle.
Use a known safe/low chip load number (2% in woods 4% in plastic).
Test Feed=(Diameter)*(safe chip load)*flutes*RPM
e.g. 1/4" 2 flute in wood at 11,400 RPM - 0.25*0.02*2*11400 = 114 IPM
All test cuts should be at 1 diameter deep per pass.
If the tool squeals than your RPM is too high. Try reducing RPM, recalculating for feed, and test again. Might need to switch to a smaller tool if you can't get the cut to not squeal at your lowest RPM.
In general tools 1/8" and smaller are not going to squeal at all at anything other than absurd RPMs (100k).
Feed
Now that we have a good know RPM we can calculate for feed. Be careful when looking at chip load numbers. I have seen them listed as both total and per flute depending on manufacturer.
Feed = (total chip load) * RPM.
e.g. 0.004 total chip load at 11,400 RPM - 0.004*11400=45 IPM
Real World
Now lets talk about the real world where we don't have perfect materials, machines, and tools. Deflection, runout, material variability, tool quality/geometry, etc will all effect the best feeds and speeds you can use. I'll run through the basics of a couple common factors.
Deflection
Deflection can be a huge limiting factor in proper feed/speed. Deflection is basically the tool or machine bending into the cut to due to the cutting forces. The weaker the components in the cnc the more machine deflection in the cut. This is why you see metal milling machines made out of cast iron with small work areas.
A quick test to see how much deflection you have is to make 2 cuts with a small gap between them. The cuts should be in alternating directions leaving a small gap where they would meet. Think of it as a straight line cut from each end toward the middle. If you have deflection then you will see that the edge of the cuts don't line up. They will be offset by the deflection. The larger the tool and the more aggressive the cut the higher the machine deflection will get.
Runout
Runout is how much eccentricity ("wobble") the tool has while rotating. Think of the bit rocking side to side as it rotates. This is usually due to poor collets or routers/spindles not having proper mating surfaces or bad bearings. The more runout in the system the worse your cut quality will get and will limit your feed. It can also limit the minimum size tool you can use and shorten the life of the bit. You may also notice that your tools are cutting larger than spec. This could be due to a poor tool but a perfect tool in a machine with runout will cut larger.
Material variability
Graded metals are usually pretty uniform. Plastics and woods are not and this means that even on the same machine your feed and speed may need to change.
For plastics things like the manufacturers mix, cast or extruded, or even temperature of the material can all change how the material machines.
Wood has a LOT of variables. Grain structure, moisture content, and silica integration are a few of the issues that come to mind.
End result
What this basically all comes down to is that while chip load numbers can be a good starting point they will usually not end up being the sole factor in getting the proper feeds and speeds. The best thing to do is take those numbers and run a test. This will get you what YOUR feed and speed should be for YOUR machine in YOUR material. We recommend running a "zigzag" test cut using your starting numbers with increases in feed at each "V". I would go into more detail on this but that's a whole other post (and this one is already quite long). A lot of this is covered in more detail on our site but I don't want to post link here as we sell bits. Another good resource for this is CNC cookbook (Link).
Acceleration
As to your question on the slow downs. This is the effect of acceleration and look ahead in the controller. Basically the software is looking at the upcoming curve and calculating how much it must slow down to keep the cut accurate. It does this because you don't want the machine to slam the tool around as fast as it can. That would be bad for the machine, bad for the tool, and give a poor cut. A good way to think of it is a car taking a sharp turn. You wouldn't want to take that turn as fast as your car could go. You slow down to take it safely and smoothly. This can obviously be changed although I don't know if you have access to this in the shark controller.
Hope that helps. If there is anything I can expand on or anything else I can help with please let me know.
John Torrez
Think & Tinker / PreciseBits
Think & Tinker / PreciseBits