Before we start milling away our stock we first need to get down to the required depth.
This is not a problem with external features when we can plunge outside.
When machining closed pockets, however, we need to find a way to get down to the machining depth first.
As usual there are several ways to get the job done. The plunging methods listed here are not ordered by their preference.
For various machining operations on different materials some may be more preferable than others.
Straight Plunging into a larger Pre-Drilled hole
This is one the best ones in my opinion. Very few machining modes can compete in effectiveness with drilling and this method will get you the best combined tool life on most materials and (in case of many deep pockets) the least machining time, even when tool change time is factored in.
We all have heard hundreds of times that when chatter is happening during machining we should simply reduce our feed rate. The same advice we also hear for compensating for extra-long tools and unstable setups.
Let me explain why I think this is mostly incorrect.
Let’s list the effects of reducing the feed rate:
Reduces tool life.
Let me explain from my own experience and research i have done each of these points and a simple single way to avoid the the adverse effects of chatter.... ...Read More
I notice when CNC Speeds and Feeds questions come up people often suggest my HSMAdvisor Machinist calculator. A referral by a satisfied customer is the best referral in my opinion. Thank you to everyone doing this great favor to me and my prospective users!
Other times users of HSMAdvisor question speeds and feeds it generates and instead of going to me, they ask on forums. Which is always fine, because extremely often "wrong" results mean something wrong in users expectations or the data he feeds the calculator
In the process of discussion it usually turns out that the calculation results were correct, but because user decided to use a depth of cut or tool length, larger than he should have, HSMAdvisor compensates and gives a very conservative feed rate.
As a developer of a very successful line of speed and feed calculators I sometimes get questions like : "I calculated speeds and feeds for a conventional toolpath. Got 5.5 cubic inches MRR(Material Removal Rate). And then I calculated S&F for the same endmill with HSM parameters turned on and got almost the same amount of MRR! What is even the point in using HSM parameters?" -they ask.
I would like to clear some things up for my friends. In this article I will explain exactly WHY HSM machining is better and HOW to achieve better productivity and tool life.
For starters here are the main features of a HSM-capable cutter:
As usual there are several components of HSM that need to be present in order for it to work to its fullest. These are:
a) Machine b) Tool c) Workpiece geometry d) Workpiece material
I intentionally did not number these as each one of those is equally important.
A few days ago one of FSwizard:PRo users questioned me over how FSwizard works.
The way SFM calculates seemed off to him.
As a result i made a quick sketch for him, that i thought i would share here.
Omar was asking me how come SFM seemed wrong for a 1" dia ball-nose cutter when making shallow depth cuts.
The sketch above shows exactly why.
On the left part we see a cutter engaged into the material to the depth equal to its corner radius. At that depth the maximum effective diameter is achieved. So an old good RPM=4xSFM/Dia formula would apply.
But at shallower depths, effective diameter of the cutter is reduced.
At 0.1" depth of cut, effective diameter would only be around 0.6"
In fact it goes to zero at the very centre. So a higher RPM will be required to achieve the recommended cutting speed.
In the same thread i also explained how DOC/WOC balancing works.
Since surface milling is more than half of what i do for a living, I decided to share some of my tips on that topic.
Generally you want to create a continuous toolpath that does not change directions too often.
Changing directions slows the machine down and reduction in feedrate affects deflection of the cutter. Different deflection means you get gouge marks on your surfaces.
When you have a long narrow piece its better to go along the long side to save on time and machine wear. Also going along the longest side reduces the number of direction changes you will have to make
When milling cavities you need to first rough, then semi-finish then finish.
Leave 15 thou after roughing, 3 thou after semi-finishing and finish to zero. All with progressively smaller tools. 5 thou stepover will give you very good finish on most ball mills 3-5 thou chiploads are very common for surface finishing.
Ball mill will always give bad finish on shallow areas- the center is not cutting, but dragging around. Also straight portion of the flute acts as a wiper and reduces scallop that the ball portion creates.
This is why going from top to bottom is safer and yields better surface finish.
The closer the wall taper angle to the taper of the flutes the better finish you will get.
There is another reason for always trying to go from top to bottom.
When taking material top to bottom you engage stock closer to the tip of the tool.
It makes cut more stable. It is more safe because you are less likely to bury the tool in stock unexpectedly. Do not go from climb milling to conventional UNLESS you need to save some rapid time. Pick up only climb milling and you are good to go. Changing from climb to conventional will cause tool to deflect away from the work on climb and into the work during conventional pass. You will see zebra marks all over your surfaces.
Lately there have been a lot of really interesting HSM topics on PracticalMachinist forums.
In one of them a guy who owns his own resharpening business posted a video of his endmill milling a block of D2 hardened to over 60 RC. The forum topic is located here First try on D2 62Rc(video)
Here is his post so you know what we are talking about:
In an effort to perfect our speeds and feeds while hardmilling, this is the first try. Its not right yet, but far from a failure. I apologize for the language at the end, but I do not edit my videos. The endmill was a reground garr VRX at .353 diameter. Parameters were 750 sfm, .018 radial, .300 axial and .004 ipt. The next run will be at 650 sfm, .006 ipt using a mist sprayer. Also, any small areas will be blocked off to be ran at lower speeds to allow cooling time for the cutter. Just a note for anyone using a Mag Fadal, The E-stop button is not quick enough, use feed hold. The endmill was badly worn on the corners, but not broken, and will be resharpened and used again.
In the ensuing discussion i posted my own take on how and why HSM works
HSM works in many ways.
1) Reduced cutting time per edge per revolution allows it to cool down more. 2) Chip thinning allows to increase chipload (advancement per tooth per revolution) 3) Increased depth of cut combined with shallow radial positively affects deflection. Tool bends less as it is more rigid towards the tool holder. 4) Higher cutting speed actually reduces cutting forces as heat generated in the cutting zone makes it easier to shear off a layer of metal. Yet because the time of contact is so small, most of the heat is carried away with the chip. 5) Higher RPM also allows to get rid of hot chips faster thus further reducing heat transferred to the tool. 6) Higher feedrate actually reduces relative cutting speed. 7) At high axial engagements more than one flute is in contact with the workpiece at different points along the axis of the tool. This too helps combat vibrations and chatter. 8) You are using more of the tool than just its tip, so technically you can do more work with one tool before it gets dull. 9) lastly it looks cool as hell and is very impressive. Whenever we know visitors or bosses are coming we try to make sure some HSM is going on even if application does not merit that I am not sure if the air that is moved by the endmill is doing much, but i suspect he didn't mean exactly that.