Do you have a question or comment concerning the operation of your Haas machine? Do you need help with a tough programming task, or want to know a better way to produce your parts? Maybe you have a better way to do something and want to share it. Check out the Technical Forum menu below for the right solution - or the right link!
Get the latest Haas Automation has to offer!
The Haas Resource Center website is here to make sure you stay up-to-date on the latest Tip & Tricks. Your Source For Routine Maintenance, "How To", Manuals & Documentation, Repairs & Service and Drawings & Diagrams.
Everything you need to know - and then some - about tooling and workholding on Haas machines.
Download this PDF document: Tooling and Workholding
First, a note of caution: Before placing any type of workholding on your machine table, be sure that the table is CLEAN and free of chips and other debris. Chips and other debris caught between a fixture and the machine table will damage both. Swarf caught between the fixture and table can cause the fixture to rock, and the parts machined will be inaccurate. Also make sure that whatever you set on the table is clean and free of debris.
Always rub the locating surface with a honing stone. This will ensure that the locating surface does not have any burrs or dings that may damage the table. If you plan to leave your workholding on the table for any length of time, a light coat of rust-preventive oil or WD-40« will help keep your table and workholding free of rust and corrosion.
The first thing to determine when you're setting up a Haas CNC mill is how you want to hold the workpiece on the machine. There are three basic types of workholding used in milling operations: vises, clamps, and chucks. The most common method of holding a workpiece for machining is a mill vise. For precision work, the vise must be set so that the clamping surfaces are parallel to the X or Y axis. This is done using an indicator. The following simple procedure makes it quick and easy to indicate a mill vise.
Tip: Use a soft or dead blow hammer to tap the fixture or vise into position. Using a ball peen hammer or other hard object may damage the fixture.
Make sure, when locating a part in a mill vise, that you center your part in the vise. You don't want a large portion of the workpiece hanging off the side of the vise. This will cause the movable vise jaw to twist and pinch the workpiece, greatly reducing the clamping force. If you try to drill a hole in the overhanging material, the Z-axis thrust may cause the material to push down at the drilling point and push up on the other side of the workpiece. If it is necessary to drill through a workpiece that is held in a vise, use step jaws. Step jaws allow you to locate the workpiece up, off the bottom of the vise. This will provide clearance below your workpiece so you can drill through without drilling into the vise. If you only have hardened steel jaws without a step cut in them, you can use a set of parallel bars inside the vise to set the workpiece on to keep it off the bottom of the vise. Always verify that the parallel bars are the same size to ensure that your workpiece is sitting flat
TIP: Most precision mill vises have a key slot and keys on the locating surface. Since all Haas milling machines have precision T-slots machined and lined up with the X axis, you can use the keys on the vise to locate the vise in the T-slot. This will locate your vise square to the table. If your vise doesn't have keys, you can make a sub-plate for the vise with keys or dowel pins on the bottom to locate in the T-slots. On the top, you can cut holes for attaching the sub-plate to the machine table, and tap holes for attaching the vise to the sub-plate. Locate the sub-plate in the T-slots and bolt it to the table. Set the vise on the sub-plate and indicate it as described above. Now, every time you use that vise, just locate the sub-plate in the T-slots, bolt it down, and you're ready to go. For high-precision work, you will still have to check the indication and make small adjustments.
When using clamps to hold a part with downward force, ALWAYS make sure that the clamp is lower where it contacts the part and higher in the back. Most downward-force clamps use a jackscrew or serrated block that meshes with serrations on the clamp, to support the end of the clamp opposite the end making contact with your part. The serrated end of the clamp must be higher than the contact end of the clamp. If it is not higher, the clamp will make contact with the edge of your part and not the top. This will greatly reduce the amount of clamping force holding the part, and probably create a dent at the intersection of the top surface and the side surface of the part. If you use the jackscrew style clamp, make sure that the jackscrew does not sit directly on the mill table. Always use a thick piece of shim stock or other material to protect the mill table from damage.
Improper use of clamp
Correctly positioned clamp
TIP: When using clamps in a production situation, periodically check the jackscrew adjustment to make sure that your clamp is still higher on the jackscrew end than the contact end. In any case, the hold-down bolt should be as close to the material being clamped as possible to transfer the maximum clamping pressure to the material.
When clamping on a cylindrical surface is required, a 3-jaw chuck mounted on your machine table may be the best way to go.
TIP: If your cylindrical surface is finished, put a set of soft jaws on the chuck. Use an end mill to machine your jaws to the exact diameter of the surface you want to clamp on. Just remember that you should always have the chuck clamped when you are machining the jaws. A piece of raw bar stock or a hex nut works well – anything that will allow the jaws to be tightened and leave room for the cutter to cut to the desired depth. This is also true if you are machining soft jaws on a mill vise. The vise should always be tightly clamped before any type of machining is performed.
In many cases, a CNC programmer has defined Z zero in the program to be at the top of raw stock. Quite often, though, raw stock is not flat or perfectly parallel to any axis.
TIP: If you need to set tool length offsets from the top of raw stock but need to have precise measurements on your tool lengths, take a light skim cut on the stock. Now you can measure your cutters from a flat, clean surface. Or you can set the tool length offsets from the fixture where the part will be sitting, then increment the Z-axis work coordinate offset to a positive value equal to the thickness of the part.
To set the tool length offsets, jog the tool down toward Z zero. When you get close, slide a sheet of paper between the tool and the workpiece. Carefully move the cutter down to the top of the part - as close as possible and still be able to move the paper. Switch to the smallest increment in the Handle Jog mode. Now slide the paper back and forth while slowly jogging down. You will begin to feel the tension on the paper. Press the OFSET key, and press PAGE UP until you get to the CLNT (LENGTH) (RADIUS) page for the tool you are setting.
Cursor to the GEOMETRY column and then down to the tool number you are setting. Press TOOL OFSET MESUR. The control will read the Z-axis absolute machine position recorded at the bottom left of the screen, and enter it as the tool length for that tool number.
TIP: When setting TLO (tool length offsets), the absolute machine position for the Z axis should be registered when the TOOL OFSET MESUR button is pressed. If this is not the case, Setting 64 in the control should be turned off.
When setting work coordinate offsets, you must locate X zero and Y zero accurately. Remember that you are measuring the centerline of the spindle to a location on a part or a fixture. If it is the edge of a part or fixture, an edge finder is the most common tool used.
An edge finder is composed of two concentric cylinders, spring-loaded together. To use it, place the edge finder in a collet chuck and offset the two halves slightly, so that there is a wobble as it spins. Then, slowly jog the part into the wobbly end of the edge finder. The edge finder will center up, and then break out of concentricity suddenly. At that point, jog the edge finder in the positive Z direction to raise it above the workpiece. Now, jog the axis you are locating by an amount equal to the radius of the edge finder. Make sure that you are on the page labeled "WORK ZERO OFFSET" and that your cursor is on the correct line in the G CODE (G54, etc.) column. Cursor across to the correct axis, press the PART ZERO SET button, and confirm that the entry went into the correct column.
TIP: If you are setting your TLO from the part, you will only need to set the work coordinate offset for the X and Y axes. The Z-axis work coordinate offset will be compensated for by the tool length offsets.
TIP: 1000-1500 rpm is a good spindle speed range when using an edge finder.
If you need to find the centerline of a hole or a round part feature, an Indicol is a helpful tool. This is a type of holder for dial-test indicators. It has a C-style clamp to attach the Indicol to a tool holder in the machine spindle. The Indicol also has two or three adjustable arms and a clamp at the end to hold a dial test indicator. The adjustable arms allow you to position the indicator to spin the same diameter as the hole.
To find the centerline of a hole, position your indicator tip just above the hole and manually spin the tool holder with the Indicol attached. You will be able to see if your indicator tip is spinning the same approximate diameter as the hole and how far off-center your current position is. Adjust the X and Y axes as close as possible before moving the indicator down into the hole. Once they're close, jog the Z axis down so the indicator tip is inside the hole, and adjust the arms so that the indicator begins to give a reading. Spin the indicator so that it is making contact with the surface of the hole in one of four quadrants (X+, X-, Y+, or Y-). Now, set the indicator to zero and rotate it 180 degrees. The amount of indicator movement is 2X the amount of axis adjustment needed. If your indicator moves minus 0.016, then you need to jog the axis 0.008 in the plus direction.
Now, rotate your indicator 90 degrees and reset zero. Rotate the indicator 180 degrees to find the amount and direction in which the other axis needs to be adjusted. Remember, the distance the indicator moves is 2X the distance that you will have to jog the axis to find the centerline of the hole. This procedure can be tricky on small diameter holes, but it is very accurate. You really can find the exact centerline of a hole, within 0.0001 of an inch, in each axis.
TIP: A huge time saver for finding the center of a hole or round part feature is a coaxial indicator. This indicator fits into a collet chuck, and you use it while the spindle is turning. Manufacturers claim that you can use these indicators at speeds up to 800 rpm, but the 50 to 100 rpm range works well; if the spindle is rotating too fast, it is difficult to tell which axis needs to be adjusted. A restraining arm allows the face of the indicator to remain stationary while the spindle rotates. With each rotation of the spindle, the indicator dial will show the amount it is off-center. You simply jog the machine axes while watching the indicator movement. This saves time because you can start the rotation while the indicator is off-center by as much as 0.250 inch, and you can literally dial it in within seconds.
The tool in the holder should have as much support as possible - leave only as much as necessary unsupported.
Selecting the right tool holder for the job is as important as selecting the right cutter for the job. You should always use the shortest tool holder possible for all machining applications. In addition, the tool should be set into the tool holder as far as possible. This will increase the tool holder's grip on the tool and reduce vibration. The shorter the distance from the spindle nose to the tool tip, the more rigid your setup will be. Increased rigidity means less vibration when cutting. Haas Automation, Inc. recommends that any tool holder running at 10,000 rpm or higher be balanced to G2.5, or better, at the maximum rpm. You can buy pre-balanced tool holders, but they should be balanced again with the cutter set in the holder.
TIP: Balancing tool holders will only improve machining conditions. It will prolong the life of the spindle and your cutting tools. It will also improve part surface finish and dimensional accuracy. Lower quality surface finish and spindle damage can occur if the balance of the tool holder, with the tool in it, is not within the G2.5 specification.
TIP: If your situation requires running the spindle at speeds in excess of 10,000 rpm and balancing the tool holders is necessary, avoid using endmill holders with setscrews. Endmill holders will not allow the cutter to run true (concentric with the spindle), due to the unidirectional clamping force applied by the setscrew. The best types of holders for high-speed use are shrink-fit holders, collet chucks with balanced nuts, and collets or hydraulic collets. These types of holders will apply even clamping pressure on the tool, so that TIR is almost zero.
TIP: For high-speed operation, round shank tooling should not have Weldon flats. Weldon flats will cause imbalance due to the uneven weight distribution. The tool length extending from the holder should be as short as possible.
When selecting cutting tools for a job, the first thing to consider is what type of operation needs to be performed. Here is a quick description of the basic cutting tools most often used in milling operations.
A drill is used to create a round, cylindrical hole in a workpiece. Drilled holes can be "through holes" or "blind holes". A "blind hole" is not cut entirely through a workpiece. Quite often, an engineering blueprint will specify a drilled hole to be drilled to "full diameter depth." This means that the hole diameter must be a specified depth without regard to the angled tip of the drill. When you measure your tool length offset, you are measuring the length of the drill and its tip. So how deep do you drill the hole so that the full diameter depth is correct? Well, you need to know how long the drill point is.
TIP: The length of the drill point is determined by the tool point angle and the drill diameter. You can calculate the length of the drill point by multiplying the drill diameter by a constant; the value of the constant depends on the drill point angle (most standard high-speed steel drills have a tool point angle of 118 degrees).
For a drill point angle of:
Multiply the drill diameter by:
Using these constants allows you to calculate the drill point length within a few thousandths of an inch.
A center drill is a small drill with a pilot point. It is used to create a small hole with tapered walls. When a hole's location must be held to a close tolerance, use a center drill first and then use a twist drill to finish the hole. The tapered walls of the center-drilled hole will keep the twist drill straight when it begins to drill into the workpiece.
TIP: Many machinists use this rule of thumb: If the tolerance of the diameter of a center-drilled hole is not critical, drill as deep as you want this diameter to be. With a standard, 60-degree center drill below 0.375-inch diameter, the hole diameter produced will be close to the depth you drilled. With larger center drills - 0.375 inch and above - the depth-to-diameter ratio becomes larger, so you could be off by as much as 0.080 to 0.100 inch.
A reamer is designed to remove a small amount of material from a drilled hole. The reamer can hold very close tolerance on the diameter of a hole, and give a superior surface finish. The hole must be drilled first, leaving 0.005 to 0.015 inch of stock on the walls of the hole for the reamer to remove.
TIP: The ideal situation for hole size accuracy and location when reaming is to process the hole with the following steps: the hole is first drilled, then bored, then reamed.
TIP: Stock allowance for a reamed hole will depend on the size of the hole. A general rule is:
for holes less than 1/2"
for holes greater than 1/2"
stock of less than 0.0150" on diameter
stock of 0.030" on diameter
The type of workpiece material and the method used to create the hole will affect the stock allowance.
A reamer produces the best, most uniform surface finish when it is fed into and out of the hole using the G85 (bore in, bore out) canned cycle. Many people try to save time by using the G81 (drill) canned cycle, which will feed into a hole and rapid out. It is quicker than G85, but will usually leave a helical swirl mark on the cylindrical surface of the hole. Although this swirl mark is only a cosmetic flaw and doesn't affect the size of the hole, the appearance of the hole may be rejected by some customers.
A tap is used to create screw threads inside of a drilled hole.
NOTE: Great care must be taken when using a milling machine to perform a tapping operation.
TIP: If you are using a machine with rigid tapping, feedrate (in inches per minute) = thread pitch x revolutions per minute. Also, you should never tap more than 1.5 x the tap's major diameter. Threaded connections will not increase in strength if the contact length is more than 1.5 times the diameter of the fastener. If you need threads that are deeper, machine tap them first and hand-tap them to finished depth. If you tap deeper than 1.5 x the hole diameter, your chances of breaking the tap increase dramatically. Chip control becomes a problem. When tapping blind holes, always drill as deep as possible to avoid packing chips below the tap. Using a spiral flute tap will bring the chips up, out of the hole. To further reduce tapping headaches, make sure all holes to be tapped are free of chips, and use a tapping fluid specifically designed for the type of material you are cutting.
TIP: Tap drill size is the size of the hole required for a specific tap. For 75% effective threads the formula that will determine the correct drill size is:
D - 1/N, where
D = major diameter of the tap and
N = number of threads per inch
A tapped hole with 75% of thread depth has only 5% less strength than 100% thread and takes only 1/3 of the cutting force of a 100% thread.
An end mill is shaped similar to a drill, but with a flat bottom. It is used primarily to cut with the side of the tool to contour the shape of a workpiece.
TIP: Programming an end mill to cut contour or pocket tool paths using cutter compensation (G41 and G42) allows you much more flexibility in adjusting the size of machined features. Using cutter compensation allows you to adjust the amount of stock removal. As an end mill wears, minor offset adjustments allow you to make every part the same size. You may also use a different size end and have the machine cut the same part features as with the end mill originally programmed for that tool path.
A bull end mill is the same as a regular end mill except that there is a radius on the corner where the flutes meet the bottom of the end mill. This radius can be any size up to one-half of the tool's diameter.
TIP: Bull end mills are effective for producing a corner radius between a wall and a floor on a given part feature. They also add to the strength of an end mill. When machining hard, tough to cut materials, the sharp corners on a standard end mill tend to chip and wear faster than an end mill with a corner radius. The radius on a bull end mill provides a more gradual shearing entry in to the work piece.
A ball end mill is a bull end mill where the corner radius is exactly 1/2 the tool's diameter. This gives the tool a spherical shape at the tip. It can be used to cut with side of the tool like an end mill.
TIP: The primary purpose of a ball end mill is to machine lofted surfaces. The spherical shape of the tool is able to move along any undulating surface and cut anywhere along the cutter's "ball end." As a ball can roll over a surface, a ball end mill can be used to cut any such surface.
An insert end mill is the same as a standard end mill but with replaceable carbide inserts.
TIP: Insert end mills are designed to remove metal at higher rates than solid carbide. They come in a large range of diameters and are able to cut at a deeper depth of cut. This is fantastic but, when using these cutters, it is a good idea to calculate the horsepower required to make a cut. Piece of cake on your Haas control: There is a button on the front labeled "HELP/CALC." Press this button once to get the Help menu, press it again to get the Calculator functions. Use the PAGE UP/PAGE DOWN keys to scroll between three pages: Trigonometry Help, Circular Interpolation Help, and Milling Help. Each one of these pages has a simple calculator in the upper left hand corner. On the Milling Help page, you can solve three equations:
With all three equations, you may enter all but one of the values and the control will compute and display the remaining value. To calculate the horsepower required for a cut, you must enter values for RPM, feed rate, number of flutes, depth of cut, width of cut, and choose a material from the menu. If you change any of the above values, the calculator will automatically update the required horsepower for the cut you intend.
The next thing to consider when choosing cutting tools for a job is what material you are going to cut. The most common materials cut in the metalworking industry can be divided into two categories: non-ferrous and ferrous. Non-ferrous materials include aluminum and aluminum alloys, copper and copper alloys, magnesium alloys, nickel and nickel alloys, titanium and titanium alloys. Common ferrous materials include carbon steel, alloy steel, stainless steel, tool steel, and ferrous cast metals like iron. Non-ferrous metals are softer and easier to cut, with the exception of nickel and titanium. Ferrous metals, on the other hand, are generally harder in composition and tougher to cut.
Cutting tool material is one of the biggest decisions you'll have to make when choosing a cutting tool. Most all of the cutters described above are available in three basic materials: high-speed steel, solid carbide, and carbide insert style. Almost all of the basic cutting tool materials can be used to cut almost all materials. It really boils down to performance. High-speed steel cutting tools have very high toughness but lack wear resistance. Carbide, on the other hand, has a very high wear resistance but chips and breaks easily. Carbide will always be able to cut materials at higher speeds and feeds, but is more expensive. Carbide insert cutting tools are very useful in high-production situations because the inserts are designed with multiple cutting edges on each insert. When they become worn out, you index the inserts to the next cutting edge, and when all cutting edges are used, you only replace the inserts and not the whole tool.
TIP: If you are using a high-speed steel drill, always use a center drill to get the hole started. Then drill the hole. This will ensure that the drilled hole is in the correct location. If you are using a carbide drill, it is not necessary to center drill first because carbide drills are ground with a self-centering tip. Using a carbide drill to drill a hole that is already center drilled will damage the drill. The outer cutting edges will contact the tapered walls before the tip of the drill begins to cut. This will shock the outer cutting edges and cause the drill to chip. Carbide drills must begin to cut at the tip before the outer cutting edges.
Each one of these cutting tool materials is available with a variety of different coatings to enhance their performance. The three coatings most widely use today are titanium nitride (TiN), titanium carbonitride (TiCN), and titanium aluminum nitride (TiAlN). TiN coating is easily recognized by its gold color. The advantages of TiN coating are increased surface hardness, increased tool life, better wear resistance and higher lubricity, which decreases friction and reduces edge build-up. TiN coating is mostly recommended for machining low alloy steel and stainless steel. TiCN coating is gray colored compared to TiN, and even harder. Its advantages are increased cutting speed and feeds (40% to 60% higher compared to TiN), higher metal removal rates, and superior wear resistance. TiCN coatings are recommended for machining all material types. TiAlN coating appears gray or black and is primarily used to coat carbide. It can work at very high temperatures, up to 800 degrees Celsius, which makes it ideal for high-speed machining without coolant. Pressurized air is recommended to remove chips from the cutting zone. It works well on hardened steels, titanium and nickel alloys, as well as abrasive materials like cast iron and high silicon aluminum.
When selecting end mill tools, the number of flutes, or cutting edges, is an important factor. The more flutes an end mill has, the smaller, or shallower, the flutes are. The solid center section of an end mill is approximately 52% of the end mill's diameter on a two-flute end mill. The center section of a three-flute end mill is 56% of its diameter, and an end mill with four or more flutes has a center section that is 61% of its diameter. This means that the more flutes an end mill has, the more rigid it will be in the cut. Two-flute end mills are recommended for soft, gummy materials such as aluminum and copper. Four-flute end mills are recommended for harder, tougher steel materials.
Cutting speed refers to the speed at which the cutting edge of the cutter moves with respect to the work, measured in surface feet per minute (SFM). Feed is the rate at which the work moves into the cutter, measured in inches per minute (IPM) (or millimeters). Feeds and speeds affect the time to finish a cut, tool life, finish of the machined surface and power required of the machine. The material to be cut and the material of the tool mostly determine the cutting speed. To calculate the proper spindle speed in revolutions per minute (RPM), multiply the suggested SFM by 3.82 and divide that product by the diameter of the cutter being used. 3.82 is a constant factor used for transposing SFM to RPM. The feed rate depends on the width and depth of cut, the finish desired and many other variables. To calculate the desired feed rate, multiply feed per tooth by number of teeth and spindle RPM.
TIP: To find the right speed for any task, refer to the Machinery's Handbookę or other reference. Most cutter manufacturers can provide general guidelines for their cutters based on the material to be cut. Many of them will even come to your shop to see the exact application and make suggestions for proper cutters, coatings, and cutting speeds.
TIP: Although manufacturer references for tool speed and feed are provided for your convenience, they are intended for reference -- as a starting place to cut. In many situations the numbers given are for ideal conditions, and they will not always work. Experience will be valuable to tune the cutter to the conditions of the cut. Chatter and vibration may occur; to overcome these conditions, alteration of the speeds and feeds will be required.
TIP: The Haas Control has as a standard feature a calculator that will assist the operator by doing calculations for trigonometry, circular interpolation, and milling. To access this feature, press the HELP/CALC button twice, then PAGE UP or PAGE DOWN to the calculator you want to access. Enter the prompted data and the control will do the math for you.
Setting up a CNC milling machine to produce excellent quality parts in the shortest possible time requires two things. The first is a lot of common sense. The second is thorough knowledge of all the topics discussed in this article. There are many excellent sources of information on all of these topics. The Haas Automation Applications department can answer all of your questions regarding Haas machines and the specific problems you may have with a machining application. In addition, cutting tool manufacturers can provide answers to questions about their products. Lastly, the Internet is a vast source for information on any subject.
The Haas control has features that allow the user to monitor and control machine function by recording and storing data about the tools the machine is using. The control monitors tools according to tool number and records the spindle load, feed time and usage for each tool, storing this information for the user's convenience.
TIP: The Tool Load page is located in the Current Commands display (when in Current Commands, any mode, PAGE UP once to the Tool Load data screen). Setting 84, Tool Overload Action, determines the machine's response to tool overload. There are four choices for Setting 84: Alarm, Feed Hold, Beep or Auto Feed. When spindle load conditions exceed the value entered in the LIMIT% column on the Tool Load screen, the machine will respond accordingly. If there is no limit set for a tool, there will be no response by the machine.
Setting 84 can be used to prevent many common problems that occur during machining. For example:
Cutters and inserts wear, and an increase in spindle load is one result of this. Monitoring spindle load helps the operator know when it's time to change the cutter or insert.
Insufficient coolant flow may cause galling or welding of material or swarf onto the tool, which will inhibit chip evacuation and impair the cutting action of the tool. This also results in increased spindle load; having the machine monitor load is useful in this situation as well.
An uneven depth or width of cut will increase the spindle load only during certain parts of the cut. Selecting Auto Feed in Setting 84 will reduce the feed rate of the machine, to maintain a specified maximum that is set on the Tool Load page. Parameters 299, 300 and 301 control the amount of reduction and recovery time.
TIP: Keeping a tool in tip-top condition can yield higher production rates. You can track the performance of a specific tool over time. Once you know the number of times a tool can cut a part and still maintain its usefulness, you can use this information to limit the number of uses of that tool. For example, if you know that a tool will fail after 27 uses, then on the Tool Life screen (Current Commands display; PAGE UP twice) you would enter 25 or 26 in the Alarm column. After 25 or 26 uses, the machine will generate Alarm 362, Tool Usage Reset. At this time the operator can press RESET to clear the alarm, change the inserts or the tool and zero the accumulated tool usage number in the Usage column on the Tool Life page.
TIP: To clear the values that are stored in the Tool Load and Tool Life screens, move the cursor to the appropriate line and column, then press the ORIGIN button on the keypad. If you want to clear all of the data in a column, move the cursor to the top of the column that you want to zero out, then press the ORIGIN key.
The Haas Tool Rack System mounts to the back of the machine, allowing popular tools to be kept within easy reach. The tool rack measures 45" x 19" and fits most vertical and horizontal machining centers.
The system comes with one rack and storage box, and additional tool trays and tool bins can be purchased separately.
Maximum weight per shelf is 120 lb.
Vertical space: Six 40-taper trays or five 50-taper trays can fit on the rack with empty tool holders.