Computer-Controlled Machining

Introduction

Computer controlled Machining, as a word suggests is the is machining process like milling, drilling, finishing, engraving etc by controlled motion of the tool over the workpiece. The motion is controlled by the code which is called G-code and is generated by the CAM software or manually and is pushed through to machine via CNC software in the computer.

CNC machine and the process for fabrication

CNC stands for Computer Numeric Control. As mentioned earlier, Computer is the key part of this type of machining involving different softwares at different steps to design, process the data and finally operate the CNC in controlled way. There are different types of CNC depending upon its axis. It can range from 2 axis to 5 axis. The one we are using is 3 axis CNC. The general process from designing to cutting is explained below.

First thing you need to do is come up with design idea, do some sketch in your sketchpad to have clear idea of how you are going to make the product.

Generate of the digital design file in 3D or 2D in CAD(Computer Aided Design) software like Solidworks, CATIA, Fusion 360, Rhino, etc. If you want to do 2D machining, softwares like Illustrator, inkscape, are also enough to create vector file like dxf. Such are used in engraving logos, characters etc.

After the file is generated, Import the design file into the CAM software like VCarve-pro, SolidCAM, Fusion 360 CAM, CAMWorks.

Set the tool, cutting parameters like pass depth, spindle speed, step over, feed rate etc, select the operation and type of tool movement in the CAM software.

Simulate in the same CAM software to see whether the tool movement is according to the input.

Export the G-code as per the machine, for the machine that we are goint to use, it is sbp file for Shopbot CNC machine. Different machine require different output, hence export the toolpath according to the suitable file that is required by the machine to operate.

Import the G-code in machine interface software, set the desired tool in the spindle.

Set the workpiece over the CNC bed, clamp it firmly.

Set the datum X,Y and Z position, make sure everything is OK and start the process.

Remove the clamps and take out the part and post process or directly use to assemble to make the final product.

The basic difference between the CNC milling and CNC router is the material that it can machine. CNC router are cheaper and do not have heavy body as CNC mill and can process wood, composites and soft metals at most, like aluminium. The machine that we are going to use is a CNC router from shopbot with bed size of 105"x 49"x 8". The machine is mainly divided in two, one is the control panel with X,Y and Z movement and another is the main spindle which is controlled by the Variable Frequency Drive(VFD). We can see the sacrificial layer on the top of the bed when we are going to use it. the workpiece here can be clamped with hand clamps or the nails. There are other ways as well like wedge or vacuum suction but we will be using nails and clamps only here. We must make sure that the VFD is connected and is in control of the software when we start using it. you can know about the machine and have look at the quick start guide from this document.

Tools

There are different tools of different sizes, different shapes and different material as well which can be used per your requirement and finishing. The shank diameter depends upon the tool type and should use the collet that fits the tool. The materials used for making tools are Carbon Steel talking about the types of tools, High-Speed Steel (HSS), Solid Carbide, Ceramics, etc. Types of tools are:

End Mill: Generally used. used to cut from end as well as sideways
Face Mill: Can be used only to cut from the end face. Used to create a flat surface
Drills: Used to make a hole and can't be used to cut sideways
Fly cutters: for smooth finish along the flat bottom surface
Taps and thread mills: To make screwed hole for fittings
Reamers: To make a smooth surface finish

Types of End mill

Square end mills: They are the most common ones and can be used for many milling applications, including slotting, profiling and plunge cutting.
Corner-radius end mills: They have slightly rounded corners that help distribute cutting forces evenly to prevent damage to the end mill and extend its life. They can create flat-bottomed grooves with slightly rounded inside corners.
Roughing end mills: They are used to quickly remove large amounts of material during heavy operations. Their design allows for little to no vibration but leaves a rougher finish.
Tapered end mills: They are center-cutting tools that can be used for plunging, and are designed to machine angled slots. They are generally used in die-casts and molds.
Ball end mills: They have rounded tips and are used to mill 3D shapes or rounded grooves.
T-slot end mills: They can easily cut accurate key ways and T-slots to create working tables or other similar applications.
Straight flutes end mills: They have a zero degrees helix. They work well for materials where the lifting effect of a spiral flute might cause unwanted results, such as wood, plastics and composites. For those materials, the straight flute minimizes the fraying of the edges and provides better surface finishes than helical general purpose end mills.

Chip removal in different shaped mills

As your CNC router spins the cutter clockwise, the helical direction of the flutes determines if chips are ejected towards the top or bottom of the workpiece. Upcut end mills are the most conventional ones, pulling the chips away from the material, which is a very important feature for most milling operations on many different materials. It has a downside if you want to cut laminated materials since it leaves a poorer surface finish on the top of the workpiece. A downcut end mill has the advantage to push chips down, leaving a cleaner cut on top, but then it will also fray the bottom edge.

Combine an upcut and a downcut and you have a compression cutter, where the flutes are carved one way for the bottom half of the flute length and the other way at the top. That feature makes them a very good candidate to cut plywood, composites, and laminates. Try to use one to cut a sheet of plywood in one pass, and you should obtain cleaner edges on both sides.

Flutes of the end mill

Flutes are the deep spiral grooves that allow chip formation and evacuation. They are the part of the end mill anatomy that create those sharp cutting edges (sometimes referred to as “teeth”).The number of flutes on your end mill is a crucial parameter that depends mostly on the material you want to cut and on the capabilities of your machine. Indeed, the number of flutes on your end mill will impact:

The feed rate of your machine
The surface finish of your piece
The ability of the tool to clear chips

Feed rate is indeed directly linked to the number of flutes of your end mill: if you add flutes, you will have to increase the feed rate, or decrease the rotational speed of your spindle, to keep a constant chip load. So depending on the speed capabilities of your CNC machine and of your spindle, you might have to choose an end mill with less/more flutes. Secondly, having more flutes on a tool creates smoother cuts, but it also leaves less space for chips to evacuate. Hence as a summary, we can say that fewer flutes are best at chip clearing, while more flutes create a smoother surface finish.

Safety

While working with the power tools or the machines, safety is the first thing that you need to follow. If you cannot follow the safety rules, you are not eligible to use any machines or power tools. It may sound boring and you might not think that it might not be important but, you only know when something bad happens, so in order to avoid those, you must comply all the safety rules.

Do's while working on CNC

Always ensure that you wear proper ear protection and a good pair of safety glasses when operating a CNC machine.
Ensure that your safety glasses are firmly in place every time you are closely observing the cutting tools.
Ensure that you wear suitable footwear such as safety boots at all times.
If you have long hair, ensure that you keep it covered when you operate the CNC machine.
Keep your hands away from any moving parts during machining processes.
Stand clear of the machine whenever it is operational. You should also warn any other people near the risk of being too close to it.
Whenever you are handling or passing tools, avoid touching the cutting edges.
Ensure that you turn the machine off completely and clean it whenever you have finished using it.
You should wear gloves when you are handling with workign with the workpiece but, must not wear it when you are using the computer as you may hit different buttons or wont feel the spindle tightness or whether tool is clamped.

Dont's while working on CNC

You should never wear jewelry or any loose clothing.
You should never try to reach into the machine while it’s running.
You should never put your hands anywhere on the work bed when the machine is on and spindle is rotating.
Never leave the machine when it’s not completely powered down.

Safety while wood working

Always use gloves as the chips might get inside you hands
Always use mask, mainly while sanding as the file dust while sanding may have bad impact on you health
Use Goggles as the chips my fly into your airs while operating
Use tight clothes and manage hair
You can use aprons for preventing chips getting into your clothes.
Always use shoes.

Cutting parameters

Chip Load: It is the theoretical length of material that is fed into each cutting edge as it moves through the work material
Chip Load = Feed Rate (inches per minute) / (RPM x number of flutes)
We can find different chipload standards according to material and can use to find the speed according to the tool and flutes in the tool.
Depth of cut: It is the depth which the tool removes the material in one pass. Maximum depth is the diameter of the tool, so you cannot have depth of cut more than the diameter of the tool. Higher depth of cut may decrease the time but may break the tool or reduce the tool life.
Spindle speed: It is the speed of the spindle which is given in RPM, It depends upon the material we are cutting and number of flutes. Different Speed than calculated may reduce toolpath, or induce fire which is very fatal
Step over: It is the overlap between each step. Step over depends upon the type of cut you want to have. If it is a rough cut you can keep it it lower but it can be increase according to the finishing you want. For more finished surface increase the overlap.
Feed rate: It is the lateral speed of the tool while cutting the job. Very less speed increase the job time and high speed will have bad impact in tool life or even break the tool. So optimum value should be chosen. perfect cut.

Above parameters should be chosen wisely. If the paramters are not properly chosen, the sound the tools makes while going though can be noted. In worst condition, the chips might catch fire which when passes through the duct collector cannot be controlled.

Climb and Conventional milling

Conventional milling is traditionally used on manual machines, where keeping backlash to a minimum is important. In this cutting direction, the tool cuts from a small amount of material up to a larger thickness, rubbing against the material through the cut.CNC machines, which have higher rigidity and are significantly less prone to the backlash, will use a Climb Milling process where the tool advances through material from maximum to minimum thickness. This cutting process allows the heat to leave the cut with the chip, reducing heat generation and tool wear while producing a better surface finish than conventional milling.

VCarve Pro

V-carve pro is a CAM software where the software generated the Gocode that can be understood by the CNC and operate accordingly. Different cutting parameters like type of tool, tool diameter, pass depth, stepover, spindle speed (i.e Rpm of the tool), feed rate, plunge rate are set in this software. Similarly, operations like profile toolpath, pocket, engraving, rough cutting, finishing etc along with the type of movement of the tool are also set in this software. This acts as a mediator or a communication device between CAD and machine and allow to operate the machine according to our requirement. You can find the about the software in detail in this manual. There is different operations that can be selected according to the requirement from the right toolbar shown in the figure below.

Tools were adjusted and table was cleaned ad clamping was done. The detail process is explained int he individual assignment. Then the cutting was started after zeroing X, Y and Z axes.The part was removed and filing was done follwed by testing. Dimensions were checked. Fitting was done for interlocking. We tested on 12 mm ply and the it had a tight fit on the 11.9mm gap.

Individual Assignment: Designing a big thing

I am a lazy person. Sometimes i just love to sit back and chill. I always wanted to have a rocking chair to relax. This was the perfect chance to make one for me. So I followed following process to make it:

CAD

STEP 1: Made a sketch of how it would be made. I wanted to make it ergonomically good so referred to some drawings as listed below.

CAD modification and export DXF

STEP 4: Added portions like stopper, added fillets on the sharp edges, moved the sitting area forward by 60mm comparing the CG of the chair.

STEP 5: Ply thickness was measured and the data was modified according to the average thickness. T-bones were added and 2D were exported. T-bones are the tedious thing to add, so I created a powercopy (a function/tool)to add T-bones in the CAD file.

T-bones and dogbones are needed in the assembly area to overcome the limitation of CNC that it cannot cut a sharp corner while cutting inside path due to the radius of the tool. While assembly, if the inserting part has sharp corner and the hollow part has the radius in the corner, there cannot be a perfect and tight fit. SO in order to avoid that, either the edges of the inserting shape has to be filleted or chamfered which might take a lot of time, hence, an overcut in the hollow side is done so that the edge of the mating part doesnot overlap with the corner radius.

CAM software, Vcarve pro

STEP 6: V-Carve pro is opened, first material was selected. We had 2440 x 1220 mm ply with thickness of 19mm though it was said as 18mm.
(Always measure your stock before cutting and modify the design according to it or there might not be proper fit and you may end up in loose fit or sanding a lot.)

STEP 7: Then import the dxf file by clicking on import vectors inside File. All parts are first selected and then click on the Join vectors inside edit objects keeping tolerance 0.5mm and hit ok. This will join the broken curves is they are nearer than 0.5mm.

STEP 8: After joining, its time for Nesting. We can find the nesting option in the Offset and Layout in the left side of the window. Click it and set the parameters as tool dia= 6mm, clearance= 10mm and border gap= 10mm. If you have free space you can increase the clearance and border gap to 20mm. Now, you can check the boxes like rotate parts for best fit, mirror parts and allow parts inside other according to your requirement. If your ply is not same on both side and want to use one side only, then uncheck the mirror parts. or if side doesnot matter you can check it which can give you optimized result. Similarly, if the grain direction doesnot matter you can put rotation check as low as 1 or in decimal places. If the grain directions matters you should keep it 180 or 90 depending upon your material. But remember, the lower value you keep, greater the time it will take to process as it has to check all the iterations shifting shape in steps you have entered. Allow parts inside another allows the parts to be inserted where there large amount of material to be removed and that space can be utilized to cut smaller parts. In my case, i have checked it all and kept the step angle at 20 degrees which gave the optimum result.

STEP 9: Now it is easy to group the vectors together which have common cutting parameters like inside cut and outside cut in our case. Hence group the geometries with inside cut in one and outside cutin another group. grouping is done by selecting the components pressing shift and after all are selected right click and group.

STEP 10: As we are doing profile tool path click on that option inside toolpaths which should be on the right side of the window.

STEP 11: Now select the cut depth. You can increase the cut depth to 0.2-0.3 mm more than the board thickness to make sure the tool cuts throught the material. For now we have kept it 19.3mm.

STEP 12: Select the tool. Here I have created a new tool of flat end mill of 6 mm diameter with single flute. Inside cutting paramtere, the pass depth which is deth of cut in one pass should not exceed the diameter of the tool. hence kept maximum of 6mm which shows 4 passes to cut the workpiece through. Step over is explained above and here since we dont have parallel ofset paths, any value is OK. Spindle speed is kept 12000 calculate from the chipload, and flutes. Feed rate us kept as less as 10mm/s to have a smooth cut and also since it is a single flute. and plunge rate is also kept 10mm/s.

STEP 12: Type of cut like inside of outside is selected. The part alike cavities and holes are inside cut and the parts where trimline is to be maintained are the outside cut. Curently, since we are selecting the cavities, inside cut is selected. Also climb is selected. Detail about climb and conventional is explained above.

STEP 13: Tabs are added by pressing add tabs to tool path, Mention tab length and thickness and press edit tabs. Then either you can do it automatically by entering required tabs per cutout or mannually adding. Tabs are the connections between the material to be cut out and the main workpiece so as to maintain the position and prevent moving around and hitting tool or eject out after the cut is done. These are small in size and can be easily taken out one the cut is done. Place the tabs in the flat areas where you can easily sand. Normally in automatic adiition of tabs, the software might add it in corners as well so I prefer adding it manaully in the flat areas.

Shopbot

STEP 18: First you have to load the material in place on the bed over the sacrificial layer. You might try to force slide the gantry, but it is NOT recommended as the rotation of the motor will generate the current which might not be good for the board when pushed fast. So, Open the shopbot software and turn on the machine as well.

STEP 19: Use the position controls by clicking on the yellow move button on the shopbot software and move the gantry at the back.

STEP 21: Clamping should be done by differnt processes but will be using clamps and screws in here. Nails can be added mannually as well and if there is very small area shopbot is used to mark the position of nail. You can use the process which will be explained later to mark the holes for screws. If you have plenty of area, you can use temporary clamps.

STEP 22: After everthing is in place, check the tool whether the tool is the one you want to cut with. In my case, since I was the first to cut in te group, I had to change it. Procedure for changing to tool is explained in the quickstart manual in the shobot section above. In brief, Take the collet spanner in left hand, and spindle spanner in right. Slide the collet spanner in the collet from below and lock the spindle with normal spanner. Push it away from you with left hand in clockwise and right in anticlockwise direction. which should release the tool. If you want to change the collet put a new collect in the nut until it snaps in the nut. Put it back to the spindle motor and apply opposite rotation towards you to stick the collect and nut to the spindle motor. Then put the tool inside the collet such that the shank is inside and the cutting baldes are out of the collet. First tighten it by hand so that the tool can self hold in the collet and then apply the key and spanner to tighten it firmly.

STEP 23: Now time to adjust Z axis. Take out the Z-Plate, clamp the aligator clip on the out side of spindle or on place where outer is connected. touch the plate to tool and check if green light glows up in the software. Then put the z-plate directly below the tool and press z-zero button. It should set z to zero.

STEP 24: For setting up X and Y axis, use the arrow keys to move the gantry and position it on your desired location where you want to start your work from. It is the point where V-carve has the x and y axis. For now I have set it to the edge of the board so that i can use full material. After moving the gantry, click on zero axes, click on zero x and y axis but dont touch z axis as it has already bed zeroed.

STEP 25: Now press cut part, select the file you have exported from V-carve pro, start the process. There will be a message to start the spindle.

STEP 26: Then first press green hardware switch which should start the spindle, check the spindle speed if it matches in the VFD control box, leave it for 1-2 miniutes, if it is the first cut for motor to warm up. Turn on the Dust collector and press OK on the computer which should start the cutting.

Mistakes and learnings

Chamfers should have been added on the interlocks for ease in assembly
Clearance or minimum 0.5 mm should have been given between inside cut and outside cut where there is interlock
While interlock test, if small size overlap is checked and seem ok, same is not going to happen for larger overlaps. The larger the overlaps or the lock contact area, larger is the friction and harder it is to assemble.
To overcome problem in the previous point, I added a chamfer of 0.5mm x 30 mm on either side of the contact walls and had main overlap area of the tested length i.e. 20mm.
Think many times before you cut. If cut more, it is loose and material addition is very hard. If cut less, sanding has to be dome which is very time consuming. So confirm, reconfirm and verify in small pieces before you cut final product.
In chair, human CG had to be considered, specially for rocking chair.
Should have added a datum hole which can be referred in case the machine powered down. This happened when the cutting was done. The first t-bone hole was taken as reference, X and Y positions were taken from the g-code. First tool was placed in the location, X & Y current position was entered as per gcode in the shopbot software as the curent coordinate. Z- axis was again levelled and the process was restarted.

Assignment