ME 13/113

Make sure you read all of the safety rules on this Wiki page.
The Safety quiz(Quiz 1) MUST be completed before operating any lab equipment! The Flow WaterJet, ProtoMAX WaterJet, and Laser safety tests must also be completed before any operation of said equipment.
- Quiz 1, Safety.
- Laser tutorial and safety test.
- ProtoMAX WaterJet safety test, this one is required for ME13/113.
- Flow WaterJet safety test, this one is NOT required for ME13/113.
- SolidWorks tutorials & downloads.
- Quiz 2, Lathe.
- Quiz 3, Mill.
- Quiz-GD&T, Videos.
- Quiz-Final, Final.
Click here to download the ME13/113 WaterJet & 3D-Printing files.

3D-Printer Tutorial:

Click here to go to the 3D-Printing page and make sure to watch the video and read the PLA information found here.

Laser Cutting.pptx

Laser Tutorial:

Draw the plaques perimeter and your name in CorelDraw as shown in the drawing below.

Please feel free to change the upper perimeter to anything you want and feel free to add images too.

ProtoMax WaterJet Tutorial:

Please go to this page for information regarding the ProtoMAX WaterJet and the ProtoMAX WaterJet safety test. This is section where the required ME13/113 safety test can be found.
Please go to this page for Flow WaterJet documentation and to take the Flow WaterJet safety test.
- Note: the safety tests for the two WaterJet machines are NOT the same.

ProtoMAX WaterJet Tutorial.pdf

SolidWorks Tutorials:

Once the SolidWorks tutorials are complete, zip them into one file and submit them in Canvas, please follow the instructions on CANVAS…

Skateboard_Tutorial.pdf

SolidWorks Skateboard Assignment Tutorial_Section 2.pdf

ME13/113 Drawings:

Base_Mill_Jan-2020.PDF

Trophy Base_Mill

Mandrel_Lathe_2020_Jan.PDF

Trophy Mandrel_Lathe

GD&T Overview_Base.pdf

Gear_Waterjet_Jan_2023.pdf

Trophy Gear_Waterjet

Plaque_Lasercutter_2019.PDF

Trophy Plaque_Laser Cut

MCE_logo_Jan_2020.PDF

Trophy Logo_3D-Print

Tolerancing:

How to Determine Hole and Shaft Tolerances:

The Hole Basis System and Shaft Basis System help a designer communicate the fit between two mating components. Generally speaking, one aims to achieve one of the following three types of fits.

Clearance Fit - where there is an intentional gap between the two mating parts
Interference Fit - where there is no gap between the faces, and there will be an intersecting of material will occur.
Transition Fit - neither loose nor tight as like clearance fit and interference fit (the tolerance zones are overlapped)

There are subcategories or refined descriptions of each fit, see page 18 of the document mentioned below.

Hole Basis System: In this scenario, the hole diameter is kept constant, and the shaft upper and lower deviation values determine the type of fit. In the hole basis system, the lower deviation of the hole will be zero.

Example: Nominal Size of Hole 36mm

Hole = 36.000/36.015mm

(Clearance Fit ) Shaft = 35.980/35.990mm (Maximum Clearance = 0.035mm; Minimum Clearance = 0.010mm)

(Transition Fit) Shaft = 35.990/36.010mm (Maximum Clearance = 0.030mm; Maximum Interference = 0.010mm)

(Interference Fit ) Shaft = 36.010/36.020mm (Maximum Interference = 0.020mm; Minimum Interference = 0.005mm)

Shaft Basis System: In this scenario, the shaft diameter is kept as the constant, and hole upper and lower deviation values determine the type of fit. In the shaft basis system, the upper deviation of the shaft will be zero.

Example: Nominal Size of Shaft 25mm

Shaft = 24.985/25.000mm

(Clearance Fit ) Hole = 25.010/25.020mm (Maximum Clearance = 0.035mm; Minimum Clearance = 0.010mm)

(Transition Fit) Hole = 24.990/25.010mm (Maximum Clearance = 0.025mm; Maximum Interference = 0.010mm)

(Interference Fit ) Hole = 24.980/24.990mm (Maximum Interference = 0.020mm; Minimum Interference = 0.005mm)

PREFERRED METRIC FITS EXAMPLE:

Click here: Hole Basis Systems and Shaft Basis Systems for determining tolerances between holes and shafts or for press-fitting applications:

Scroll to page 18 of 63 to Table 1: Description of Preferred Fits
If you start with a shaft of known diameter and tolerance and would like to size a hole in a mating part properly, refer to the Shaft basis column in Table 1.
Select the general fit category that you desire (clearance, interference, transition, or any other subclass of these)
Select from the options for that type of fit in the DESCRIPTION category column of Table 1. For example, if you desire a shaft basis interference fit, your description options are either (a) Location Interference fit, (b) Medium Drive fit, or (c) for Force fit, as noted in Table 1 below.
Select the corresponding Shaft Basis code designation (e.g., U7/h6 if a Force (interference) fit is desired)
Now scroll down several pages in the document until you find the Shaft Basis Clearance Fits Tables beginning on p.23 of 63.
Locate your shaft diameter in millimeters within the basic size column and read across until you locate the vertical column corresponding to the shaft basis code designation. Consider an example whereby your shaft has a diameter of 11mm, and you desire a force fit in your specific application.
Scroll down to p. 25 of 63 and locate 12 in the basic size column, note that this rows range is: 10mm<X≤12mm.
Now read across the vertical columns until you locate U7 (hole) and h6 (shaft tolerance) in the Force Fit column. You will now find the dimensional tolerance of the required Hole diameter (max and min diameters) listed as Max Diam. = 11.974mm and Min Diam. = 11.956mm.
Note that the shaft diameter is given as Max Diam. = 12.000mm and Min Diam. = 11.989mm where the upper deviation of the shaft is zero, as previously mentioned.
- Find the IT7 value by subtracting the two hole diameters; 11.974mm-11.956mm = 0.018mm or by using the IT Tolerance chart.
- Find the U-shift value associated with the U designator buy subtracting 12mm-11.974mm = .026mm.
- Subtract the U-shift value from 11mm to get the Upper Hole size; 11mm-0.026mm = 10.974mm (LMC_Housing).
- Subtract the IT value from the Upper Hole size to derive the Lower Hole size; 10.974mm-0.018mm = 10.956mm(MMC_Housing).
- The Upper Shaft size is 11mm (MMC_Shaft), since the h designator shift value is zero.
- The Lower Shaft size is calculated as follows: 11mm - (12mm-11.989mm)(This is the associated IT6 value) = 10.989mm (LMC_Shaft).
- The Upper Fit Limit can be found by subtracting the Lower Shaft size(LMCS) from the Upper Hole size(LMCH): 10.974mm(LMCH)-10.989mm(LMCS) = -.015mm.
- The Lower Fit Limit can be found by subtracting the Upper Shaft size(MMCS) from the Lower Hole size(MMCH): 10.956mm(MMCH)-11mm(MMCS) = -.044mm.
  - The two Fit Limits (Fitb) in the Fit Chart should match the Upper & Lower Fit Limits calculated in the last two steps.

Dowel Pin Hole Sizing Example:

This example will demonstrate how to properly dimension a dowel pin hole callout.

Knowns:

Pin size: 5/16", the standard series pin dimensions are from 0.3126"(LMC) to 0.3128"(MMC).
The Shaft Basis Metric Fit will be a G7 Sliding fit in this example.
- Referring to the Fitb column in the Shaft Basis Metric Clearance Fit chart, the tolerance range is from 0.005mm(TolMin) to 0.029mm(TolMax).
- Since these tolerances are clearances, they are positive values. If they were interference fits, these values would be negative.

Equation for the Hole Size: Hole Size = (HoleMMC + HoleLMC) / 2 = ((PinMMC + TolMin) + (PinLMC + TolMax)) / 2

((0.3128" + 0.005/25.4) + ( 0.3126" + 0.029/25.4)) / 2 = 0.3134"

Equation for the symmetric tolerance: (Hole Size) - (PinLMC)

0.3134 - 0.3126 = 0.0008"

Therefore the hole callout is as follows: Ø.3134"±.0008"

Geometric Dimensioning & Tolerancing (GD&T) Basics

Click here for the GD&T Basics page.

International Tolerance Standards:

Tolerance Grade Processes:

Click here for the International Standards ISO 286-1 pdf file.

International Tolerance Grade (IT): A group of tolerances that vary depending on the basic size, but that provide the same relative level of accuracy within a given grade. For example, it is designated by the number 7 in 40H7 or as IT7.
IT grades may be used with alternate prefixes which identify how the tolerance limits are distributed around a nominal value. When used with the IT prefix, IT grades do not specify how the tolerance limits are placed around the nominal value, alternate prefixes are used for this purpose. For example, if the tolerance limits are distributed symmetrically above and below the nominal value, the prefix "js" may be used. For example a part dimensioned (in millimeters) as 4 js7 is equivalent to 4 ± 0.006 (where 4 IT7 is 0.012.)
Other standardized prefixes include the letters A, B, C, CD, D, E, EF, F, G, H, J, K, M, N, P, R, S, T, U, V, X, Y, Z, ZA, ZB, ZC (for holes), and the lower-case equivalents (for shafts.) Prefix letters I, L, O, Q and W are not used to avoid confusion. Of these, the letter prefixes H and h are easiest to explain as the tolerance lies entirely on one side of the nominal size. A hole dimensioned at 4 H7 may range from 4.00 - 4.012 mm, and a shaft at 4 h7 may range from 3.988 - 4.00 mm.
ISO 286 identifies a set of preferred tolerance classes for holes which include G7, H7, JS7, K7, N7, P7, R7, S7, F8, H8, E9, H9, D10, A11, B11, C11, and H11. The set of perferred tolerance classes for shafts includes g6, h6, js6, k6, n6, p6, r6, s6, f7, h7, e8, d9, h9, a11, b11, c11 and h11.
To completely specify the fit between a hole and corresponding shaft, it is common to specify a pair of the above tolerance classes, for example H7/g6. As with all IT grades, the smaller numbers correspond to tighter tolerances. Under normal circumstances, only a small number of the possible fits are practically required, and ISO 286 identifies preferred fit combinations including these as most preferred:

ISO Tolerance Calculator
Click here to view the ASME B18.8.2-2020 dowel pin standards.

Bearing Fits:

Fits between Radial Bearings, shafts and Housing Bores.pdf

Bearing to housing and shaft example:

Load classifications are as follows:
- Light load: Pr ≤ 0.06Cr
- Normal load: 0.06Cr < Pr ≤ 0.12Cr
- Heavy load: Pr > 0.12Cr
  - Pr: Bearing equivalent load
  - Cr: Bearing basic dynamic load rating

Always refer to the bearing manufactures fit specifications!
Thin-walled housings normally require a P7 fit if the bearing is to stay stationary.
Plastic housings normally require a U8 fit if the bearing is to stay stationary.
In the case were the inner ring of a bearing is rotating and the outer ring is stationary; an interference fit is desired on the shaft because the inner ring is the one rotating. A transition fit is most appropriate for the housing bore because it will allow for easier installation as well as displacement for removal.
It will be unusual for a shaft and housing fit to be the same. One fit requires a clearance or transitional fit, the other, generally, the rotating ring, will require an interference fit. The rotating ring requires this interference fit because when applying the load to a looser fit, there would be slippage and a loss of efficiency, and eventually, surface damage or fretting corrosion. Often, vibrating or shaker-type applications vary from the above generality. Incorrect fits can cause premature bearing failure.

Example:

Housing Type: Solid, not thin walled
Housing Material: Steel
Direction of Load: Indeterminate
Loads: Normal; 0.09Cr
Bearing type: Ball
Bearing size: 30mm I.D. x 62mm O.D. x 16mm wide
Results from the Bearing Fits guide:
- Tolerances for Housing Bore: K7, this is a Shaft Basis condition with a size range from 61.979mm to 62.009mm.
- Tolerance of Shaft: k5, this is a Hole Basis condition with a size range from 30.002mm to 30.011mm.

The above values were derived as follows:

Tolerances for Housing Bore:

Referring to the Bearing Fits table 7.2 (1) Housing fits, a K7 fit is desired.
Referring to the Bearing Fits table 7.6 (2) Housing fit, column ∆dmp. The MMC of the outer diameter of the bearing is 62mm and the LMC is 62mm - .013mm = 61.987mm.
Referring to the second page of table 7.6 (2) Housing fit, column K7, the fit range is from 21T – 22L. T is an interference fit and L is a clearance fit.
- Note that the Housing needs to be designed in such a way as to never have an interference fit greater than 21µm and a clearance fit of 22µm.
The Housing MMC is derived as follows: 62mm + (-.021mm) = 61.979mm(MMCH).
The Housing LMC is derived as follows: 61.987mm + (+.022mm) = 62.009mm(LMCH).
- Note that a T designator has a negative value and a L designator has a positive value.
- Note that these two values concur with the K7 fit in the Preferred Metric Limits & Fits charts.

Tolerance of Shaft:

Referring to the Bearing Fits table 7.2 (2) Shaft fit, a k5 fit is desired.
Referring to the Bearing Fits table 7.6 (1) Shaft fit, column ∆dmp. The MMC of the inner diameter of the bearing is 30mm - 0.01mm = 29.99mm and the LMC is 30mm.
Referring to the second page of table 7.6 (1) Shaft fit, column k5, the fit range is from 21T – 2T. T is for an interference fit.
The Shaft MMC is derived as follows: 29.99mm - (-.021mm) = 30.011mm(MMCS).
The Shaft LMC is derived as follows: 30mm - (-.002mm) = 30.002mm(LMCS).

Determining Bearing Fit Limits:

To find the housing lower limit fit, subtract the bearing/shaft MMC from the housing MMC: 61.979mm(MMCH) - 62mm(MMCS) = -.021mm.
To find the housing upper limit fit, subtract the bearing/shaft LMC from the housing LMC: 62.009mm(LMCH) - 61.987mm(LMCS) = +.022mm.
- Note that these two values concur with 21T – 22L call-out in the bearing fits charts.
The shafts upper and lower limit fits can be found in a similar manner.
- 29.99mm - 30.011mm = -0.021mm
- 30mm - 30.002mm = -0.002mm
  - Thus 21T-2T
  - Note: this method will be slightly different for standard Limits & Fits because this example accounts for bearing tolerance.

Machining Speeds Charts:

Speeds for Drilling.pdf

Drilling & Reaming Speeds for Drill Presses, Mills, and Lathes:

Reduce the given speed in the above chart by 1/2 for reamers and 2/3 for Counterbores & Countersinks!

Do NOT run the conventional mills at a higher rate than 3000_RPM, ACER Lathes greater than 1700_RPM, and the TRAK Lathes greater than 2000_RPM.

How Dimensional Tolerances Impact Part Production Costs:

How much will a custom-manufactured component ultimately cost to produce? The answer depends on several factors. These unique parts are defined by engineering drawings, which are used by the design engineer to communicate all of a part’s characteristics to the manufacturer so that it can be consistently produced. The drawing contains numerical dimensions that define the size and location of every feature of the part. It also communicates other important attributes, including the material, surface finishes, fabrication methods and other industrial processes necessary to create the part. All of these variables contribute to the bottom line of total overall production cost.

Arguably, one of the most important requirements a drawing defines is the tolerance of each dimension. The tolerance defines the acceptable amount of deviation from the dimension’s nominal value. The “allowable tolerance” window can have a dramatic effect on the manufacturing method and total cost of producing the part. As a general rule, the smaller the allowable deviation, the greater the cost of manufacturing. This phenomenon is due to the fact that extremely precise dimensions are more difficult to achieve and increase the chance of rejection, rework and scrap.

Also, a “tight tolerance” could require the manufacturer to use much more expensive production methods, machine tools, inspection devices and a significantly greater amount of total processing time. This can add up to a significant amount of money if applied to hundreds of dimensions on the hundreds of custom parts that make up an entire machine. If the machine will be duplicated hundreds of times, the cost increases are exponential.

It is the designer’s responsibility to determine every dimension’s tolerance and make sure that it is contained in the drawing. Dimensional tolerances should be determined based on how the parts fit together and what the parts are intended to do. A designer should ask the question: Will the parts go together and function if I allow a greater amount of variation? If the answer is a definitive “yes,” then a larger tolerance should be allowed. From a cost perspective, dimensional tolerances should be as large as possible without impacting the assembly or the performance of the part.

Machining Operation Cost Chart

Dimensional Tolerance Cost Chart

Using a Combination Drill & Countersink (Also known as a Center-Drill):

Using Taps & Tap Selection:

Hand Taps:

Taps Are Brittle – Handle With Care! In order for taps and dies to cut, they must be harder than the materials they are cutting. This additional hardness also makes them brittle, meaning, they can be easily broken, something you want to avoid at all costs. It is always preferable to use a proper T-handle for taps rather than a wrench or locking pliers. The latter two work, in a pinch, but you must be careful because turning the tap from one side only can put asymmetrical stress on the tap, causing it to go off center, or break. Using a T-Handle keeps the force applied over the center of the tap or die, maintaining proper symmetry.

Lubricate! Although there is really not much heat build-up to speak of when had cutting threads, lubricating the cutting threads can reduce friction binding and aid in chip removal. You can use a a specialty tapping fluid, a light machine oil, or WD-40. When tapping brittle metals like brass and cast iron, lubrication is not normally needed and may cause chip buildup issues.

Take Your Time… You really don’t want to mess up a tapping job. Breaking a tap off in a hole —especially below the surface level will cause you untold frustration and possibly a number of colorful expletives! Remember, taps are very hard, so trying to drill one out can be difficult, if not extremely messy. Take your time, go slow, this is truly one of those situations where haste could indeed make waste —of several hours of your time and possibly, your wallet.

Break Up The Chips… The cutting teeth on a tap are not continuous all the way around the tap body. There are usually 3 or four cutting sections separated by a groove, called the flute, between them. Once the first full teeth begin cutting, the metal being removed may be a long strip, called a swarf, or chips. The flutes job is to provide clearance so the chips can be kept clear of the cutting teeth and pushed out the top of the hole.

It is extremely important that these cuttings be broken up to prevent jamming and breaking the tap. The best way to do this is to turn the tap in the direction of cutting until you start to feel a little binding. At this point, turn the tap slowly in reverse until you hear, or feel a ‘click’ of the chip breaking away from the material being cut. The vast majority of tap breakage can be avoided by making sure you break the chips, and the smaller the tap, the more important it is.

Spiral Point Taps:

These taps have a spiral cut with relief grooves, the spiral angle on the front cutting edges helps eject the chips and the angled edge also gives superior cutting performance. The primary disadvantage of these is they push the chips ahead of the tap–down into the hole in other words, this is not a big deal for through holes but is a bad idea for blind holes. Generally there is not a need to reverse these taps to break the chips. If you don't feel any binding, just continue to turn the tap until it goes through the material.

Using the Horizontal Band Saw:

DAKE Band Saw Manual_Reduced.pdf

When cutting short pieces of stock in the horizontal band saw, you will need to place something that is the same width as the stock at the far side of the vice (furthest side from the saw blade) so the the vises movable jaw stays parallel to the fixed jaw. Failure to do so will result in the stock abruptly moving and damaging the saw blade.

Band Saw Tooth Sizes:

Always make sure that there are at least THREE teeth engaged in the cross-section of the material!

Band saw tooth sizes.pdf

Using the DoAll Vertical Contour Band Saw:

Job Selector Dial:

Tooth Selection, always make sure that there are at least THREE teeth engaged in the cross-section of the material!

Bi-Metal Saw Blade Speed Chart:

Conventional Lathe Information & Videos:

Lathe Operations:

Swarf Hazard:

NEVER try to remove swarf with your hands, use a brush, pliers, or swarf hook!

Note: If you have swarf/chips that looks like this, the speed & feed need to be corrected!

TPG Style Inserts:

For additional TPG style insert speeds, please click here.
Please click here for Top-Notch style insert speeds, these inserts are on the TRAK lathes.

Surface Finish Chart:

Nose Radius Selection and Surface Finish.pdf

If you need to get a better idea on what these different surface/texture values look like on a real part, please ask the Lab staff to show you the Surface Comparator.
- Surface finish/texture affects friction, corrosion, heat transfer, wear and many other factors. For example, very rough surfaces help to improve the grip on parts that need to be held in the hand, but would be completely inappropriate as a bearing surface.
- Most bearing interfaces have a surface finish callout from the manufacture of the bearings, this finish is a function of bearing size and tolerance grade.
  - For a bearing of <80mm, the surface finish value is 63µ-in for a tolerance grade of IT7.
  - 32µ-in for a tolerance grade of IT6.
  - 16µ-in for a tolerance grade of IT5.
- Choosing a very fine surface finish is desired for components that are going to be highly cyclic loaded so that the comport does not fail due to metal fatigue.

RPM = SFM * 3.82 / (Diameter of part in Inches)
Feed rate in Inches Per Minute(IPM) = RPM * (Inches Per Revolution(IPR))
Depth will very with setup rigidity, length of stock, stock diameter, material type, and the machines available power.
Since most of our lathes do not have flood coolant, choose the lower SFM value in the above chart.
- If the first cut goes well you may increase the SFM value.

Speed & Feed Example:

The material to be turned is 1.5" in diameter, 6061-T6 aluminum, and the desired surface finish is 60µ-in.
- From the above chart; choose the SFM value of 528.
- From the above speed equation, this speed was calculated; RPM = 528 * 3.82 / 1.5 ≈ 1345_RPM. Please do NOT run the ACER Lathes greater than 1700_RPM, and the TRAK Lathes greater than 2000_RPM.!
- Choose a surface finish value and look up the feed rate in IPR from the Surface Finish Chart above, noting that the selected insert has a 0.015" radius.
- From the Surface finish chart above using an insert radius of 0.015" and a RMS value of 60µ-in; the feed rate is approximately; 0.0055_IPR.
- If you are using one of the conventional lathes, move the feed selector levers to the closest setting that matches the IPR value.
- If you are using one of the TRAK lathes go to the step below.
  - From the feed rate equation above, this feed rate was calculated; IPM = 1345(RPM) * 0.0055(IPR) ≈ 7.4_IPM.

Preferred Setup & Turning Procedures:

Lathe Cutting Procedure.pptx

Conventional Mill Information & Videos:

Drill Bits & End Mills:

So why use an End Mill and not a drill bit? In short, a drill bit moves up and down, an end mill moves side-to-side (Note: there are End Mills available that move in all directions).

Various End Mills:

End Mills:

- Cut rotationally in a horizontal, or lateral (side to side) direction whereas a drill bit only cuts straight down, vertically into the material.
- Are available in a wide variety of lengths, diameters, flutes and types, and are chosen according to the material they are cutting and the surface finish required for the project.
- Are the cutters of the milling world and are used for slotting, profiling, contouring and counter-boring.
- Allow for precision parts to be cut, anything from machine parts, wood engravings, sign making, plastic cutting, mold making, etc.
- For most end mill to cut properly they need to turn in the clockwise direction, looking from the top down.
- If a large burr starts to form while using an end mill, it is most likely dull or spinning in the wrong direction.

Jobber & Stub Drill Bits:

Drill Bits:

- Cut round holes straight down into the material by rotating them in a rotary drill.
- Most drill bits have a spiral groove (flutes) which give the drill bits a twisted appearance and helps to cut away material as they move up and down in the hole.
- For most drill bits to cut properly they need to turn in the clockwise direction, looking from the top down.
- If a large burr starts to form while drilling, it is most likely dull or spinning in the wrong direction.

NEVER put an End Mill in a Drill Chuck!

End Mill Cutting Speeds for the Trophy Base:

In order to calculate the cutting speed for an End Mill, take the cutting speed in Surface Feet per Minute(SFPM or SFM) and multiply it by 12/π ≈ 3.82, then divide it by the diameter of the End Mill. E.g., using a 1/4" High Speed Steel (HSS) End Mill in aluminum; RPM = SFM * 3.82 / 0.25 = 160 * 3.82 / 0.25 ≈ 2445 RPM. Please do NOT run the conventional mills at a higher rate than 3000_RPM!

These values are for Aluminum ONLY!

3/16" HSS End Mill, 140_SFM

1/4" HSS End Mill, 160_SFM

3/8" HSS End Mill, 175_SFM

1/2" HSS End Mill, 200_SFM

3/4" HSS End Mill, 200_SFM

Edge Finder:

The Edge Finder is a dynamic indicator of the location of an edge with reference to the centerline of the longitudinal axis of the spindle to which it is attached. In use, the spinning Edge Finder is moved into contact with the edge that you wish to locate. As the lower cylinder of the Edge Finder touches the edge, that lower cylinder ‘kicks’ to the left (assuming a clockwise rotation as seen from above).

When the kick is observed, the axis of the spindle and the edge of the workpiece are located 1/2 the diameter of the Edge Finder from each other. This is typically 0.500″ (0.500/2 = 0.250″) but can be different so check.
- Make certain there are no burrs on the workpiece or you will get a false edge indication. The same goes for excessive oil on the workpiece.
- Do not chuck the Edge Finder with excessive pressure, it is hollow and can be crushed.
- You should run the Edge Finder in the range of 700-900 rpm for the 1/2" diameter and 1200-1500 rpm for the 0.2" diameter.
- If possible, the spindle should be extended so that when you see the ‘kick’, you can retract the spindle and remove the Edge Finder from the workpiece. This saves wear and tear on the lapped surfaces of Edge Finder.
- View the workpiece/Edge Finder contact by aligning your eye behind the Edge Finder, at a 90° angle to the workpiece for maximum visibility of the ‘kick’.
- The working portion of the Edge Finder is the smaller diameter cylinder. This is the part that should contact the edge in questions.

Please click here for a video on how to use the Edge Finder.

Conventional Milling

Conventional Milling versus Climb Milling:

Climb Milling

Conventional versus Climb Milling Considerations.pdf

Tool changing Procedure:

Milling Machine Tool Changing Procedure.pdf

Additional Mill Information:

For more information regarding Milling & Drilling Operations, please click here.
Please click here for ME13/113 Mill Videos

Page updated

Google Sites

Report abuse