A Ramping, the VR Command and How to Tune Your Tool for Maximum Performance - March 2008

No setting in the ShopBot control software (SB3) has more influence over the performance of your CNC than the VR [Values Ramping] command. I have no doubt that you've heard about ramping before, and to many, the idea of adjusting your VR settings is downright confusing and to some, scary. There seems to be a myth that somehow you are going to permanently ruin your CNC if you adjust the ramps yourself and get the settings wrong. This article is going to dispel that myth and help you get your CNC to move and cut the way that you want under a number of different conditions. There are a number of factors involving ramp values [VR] that are too complex to convey within this column. However, it is my goal to give both new and seasoned users a glimpse into your ramp settings and how you can tune them for the type of work that you do. Keep in mind that your ability to observe how your tool moves when adjusting ramps, is the key to tuning your tool for the exact type of work that you do. It is your responsibility as an operator to tune the tool to fit the needs of your work. ShopBot did an excellent job with baseline settings, now that your CNC abilities have grown, it’s your turn to get your tool dialed-in like a pro.

So, what is ramping? Within the context of this article, ramping refers to the manner in which your tool starts, stops and regulates movement using the SB3 control software. Just to make a distinction, these are ramps in speed. I will not be discussing cutter entry ramps, where your tool moves in an XZ or YZ 3D incline into your material to reduce stress on your bit when plunging. In order to grasp many of the concepts that I will be discussing, you'll want to familiarize yourself with the [VR] command in the Command Reference PDF, found under the Help menu in SB3. You can also access it by typing HC into the yellow command box in SB3. You will also want to read, “Ramping – Detailed Explanation” starting on page 21.

Let’s first take a look at a graphical representation of a typical ramp shape, showing the speed the tool moves in relation to distance:

If you typed in [MX, 48] into SB3, your tool will start moving at XY Move Ramp Speed, accelerate according to the Move Ramp Rate you’ve set (Ramp Rate being the slope of the acceleration line), run at the Move Speed [MS] you have indicated in your part file, then decelerate at the set Move Ramp Rate to the ramp speed where it stops at 48 inches. The illustration above shows the simplest ramp shape that your tool will make.

There are things that you must consider when pondering move speed [MS] and ramps [VR]. Just as you cannot make your car go from zero to 100 to zero again in a convenience store parking lot, you cannot make your CNC go from zero to 12 IPS to zero again within 8 inches. SB3 is smart enough to not allow the tool to make these types of aggressive moves. It will look ahead and set an appropriate course of action when you ask it to do something that violates the basic laws of physics.

Working with the [VR] Command

Here are the default VR settings for a PRS Alpha CNC. These are the settings that most influence cutting. Settings for a PRS Standard machine will vary slightly, but you will be able to apply the same concepts to your tool.

The occurrence of a ramp is influenced by a number of factors, but especially by a change in the direction the tool is moving. If you set your tool to move at 4 in/sec in XY when cutting out a 24 inch square with sharp corners, then your tool will move 4 in/sec on the straight sections but will ramp the direction changes going into and out of the corners (decelerate into and accelerate out of the corner. Curved corners, circles, and arcs will trigger ramps if they are tight, but in other cases ramping will not take place if you are cutting a large enough arc or curve. We will discuss this in further detail later in the article.

But back to the [VR] Fill-in Sheet. Starting at the top of the sheet, we have the XY Move Ramp Speed (MRS). Here it is set to 0.4 inches per second. This setting essentially sets the starting speed of your tool when moving from a dead stop. It is often helpful to lower this speed value when you are machining intricate or small parts, or machining very dense materials, such as non-ferrous metals, since it will reduce cutter deflection. It is also helpful to lower this value when you are using small cutting tools under 1/16” diameter. The downside to setting this value too low is that it can start the tool out too slowly under general cutting conditions and it will take longer to get up to speed, making the tool feel sluggish. Only modify this if you need to.

The next three settings do the same as the XY Move Ramp Speed, but correspond to their indicated axes. You may find it helpful to lower both the XY MRS and the Z MRS when doing small or intricate v-carving. For most 2D and 3D cutting, it is not necessary to adjust the Move Ramp Speed.

The next four settings influence jog moves, and they are best left alone.

Let’s have a look at the next setting, Move Ramp Rate. This setting defines the acceleration and deceleration rate for ramping as a distance. It essentially tells SB3 how much room it has to speed up or slow down the movement of your tool, by two speed units (2mm/sec or 2 in/ sec). By increasing the Move Ramp Rate, you are making ramps longer and smoother. This adds a sort of cushioning effect to the tool’s movement. By shortening the Move Ramp Rate, you make tool movements more aggressive, which may or may not be desirable depending on the part you are cutting. The default 0.2 value is a good general setting. If you are doing 3D relief carving with many moves in the Z, you may want to experiment with lowering the value to 0.1 and checking the cut quality of your parts. [Tip: It is important that you have your v-roller bearings on your Y and Z axes adjusted properly to eliminate any slop and vibration that may get transferred to your cut part when doing aggressive 3D]. For most parts, the 0.2 default setting works well.

The Jog Ramp Rate functions well at the default setting of 0.2 and is best left alone.

Let’s move on to the 3D Ramp Threshold setting. This setting controls how sensitive ramping is in the Z axis when cutting 3D reliefs. The higher the value, the more responsive and less sensitive to ramping the Z, A, or B axes will be when cutting. The default is 100, I like 150 as a good general setting for most 3D files. Keep in mind that your move speed (MS) will influence 3D ramping if the Z axis cannot respond fast enough to XY movement. If you are rastering over a 3D relief and meet an abrupt wall or large change in Z height, and your Z move speed is not fast enough, SB3 will trigger ramping to occur, and this will slow down the XY movement to match what the Z axis can handle. More on this later. There are situations, where increasing the 3D threshold is very useful. If you have a relief with a lot of little moves, such as one with a background texture, where the Z has to move up and down quite a bit, an increase in the 3D Threshold can help to speed things up, provided that your Z speed is high enough where the XY doesn’t have to slow down. For most reliefs, however I have not found that increasing the 3D threshold to be beneficial. In many cases, increasing the 3D threshold beyond a value of 200 when cutting a low detailed relief can result in jerky Z moves, and in other cases not influence the movement of the tool at all. Use your best judgment, and experiment with settings for the type of work that you do.

The Minimum Distance to Check (MDC) setting works in conjunction with angular movements and basically adjusts when ramping will happen based on the tightness of the corner. It will influence ramping when very small bumps, curves or jagged features are present in your cutting file. The larger the number, the more likely you will get ramping with small curves or features. The default is 0.1 and I like to set this to 0.08 to since I often work with very intricate designs. This adjustment reduces the tendency for ramping. The MDC setting also adjusts the speed that very small circles will be cut at since a small circle is basically a continuous tight arc. Making the number smaller will mean that small circles are less likely to ramp.

The illustration below shows how very detailed 2D & 3D models can cause jagged cutting and even tool vibration, if the minimum distance to check value is set too high. The example below shows a 0.125” bit cutting a span of jagged vector nodes. The ideal cutting path is suggested as a straight line. The green areas indicate movements less than the MDC and the red areas show the 0.125” bit making a movement change greater than the MDC. Rather than over-think the Minimum Distance to Check value, set it to .08, as I have found this to be a good setting for all types of cutting.

The sharper a corner the more the tool will slow down. In a tight angle, the speed will slow to the Ramp Speed for the primary axis and type of move. With a slight angle or gentle curve, there will be a slight slowing. The amount of slowing is the Slow Corner Speed (SCS). SCS is a percentage value of your move speed (MS). The default setting is set at 65%, which I find to still be a little too fast for me. The SCS influences how fast the tool will traverse a corner in both 2D profiling and 3D profiling. I have found that anywhere from 25-65% is a good range for just about any type of cutting you will need to do. If you find that your tool is taking corners a little too quickly, then you will want to reduce the SCS value. While this is not much of an issue on a PRS Alpha, standard PRS tools can reduce the chance of lost steps by reducing the SCS, especially when cutting aggressively in sheet goods or high-speed 3D raster movements. The SCS will add a bit of cushion at the end of raster moves, and slow down your tool in the corners, drastically reducing cutter deflection. I often lower the SCS to 40-50% when cutting 2D parts, and between 30-45% when cutting in 3D, since I find that it eliminates or greatly reduces the tendency for the tool to ‘bang’ when it meets a sharp wall of a relief carving.

Specialized Settings for STOPS and KeyPad. The last few settings in [VR] define some specialized threshold settings. The Fast Stop Threshold sets the highest speed where your tool will instantly stop when you hit the Space Bar or the E-Stop. At higher speeds you will get a ramped stop and a Z axis pull up from the material followed by the router/spindle being turned off on tools with spindle control. This type of ramped stop can always be triggered via the S key. The default setting has been 3, but ShopBot has recently changed the default to .2 so that all STOP conditions will trigger the same, safe, ramped stop with Z pull-up and spindle turn-off. You can still set the value higher so that for special conditions you can have an instant stop. However, values above 3 are not recommended as this puts a lot of shock into the drive system.

The remaining two threshold settings apply for KeyPad [K or SK] mode only. They adjust how the tool responds when moving the tool around with the arrow keys. The Keypad Stop Threshold is very similar to the Fast Stop Threshold. The default is 1.75 IPS, I’ve bumped mine up a little to 2 IPS. The Keypad Ramp Rate is similar to the Move Ramp Rate, and it controls how quickly the tool will accelerate and decelerate when moving the tool with the keyboard. The default is 0.8, which I found to be too soggy. I set mine to 0.2 for crisp movement. However, some people prefer the slower response because it allows very precise small moves.

My approach to VR Settings

Now that you have a basic understanding of how [VR] settings can influence your tool, let’s talk about some of the settings that I use for different types of cutting. Generally speaking, the settings that influence the movement of the tool the most are Slow Corner Speed, and Minimum Distance to Check. Most of the time, I will only adjust the Slow Corner Speed, after I have set my values to the numbers I have suggested throughout this article. 3D cutting is a bit more involved, since dialing in [VR] for every type of 3D file you may encounter is tough. By this, I mean, running the tool as fast as I can with the best finish quality, without watching my tool beat itself to death with vibration. For most 3D reliefs, the settings I suggest in this article are adequate. Files that have a lot of surface or background texture will benefit from a higher 3D Threshold value, a lower Move Ramp Rate and a higher Slow Corner Speed. If you find that your tool sounds too rough for your liking, return the Move Ramp Rate to 0.2. If it is still happening, reduce the 3D threshold to 175 and if it is still happening, reduce the Slow Corner Speed. These settings have the most influence over 3D cutting. Additionally, since the Minimum Distance to Check also works in 3D, you may want to try lowering the value so that it is less sensitive to those little details in the background.

I want to take a moment to talk about move speeds [MS] and 3D cutting. Getting your move speed set correctly in your part file is just as important as getting your [VR] dialed in. If you set a MS, 6,3 in your file that cuts a 6 inch wide relief, cutting will not be smooth or as expected for two reasons. One, the XY speed is too fast for the size of the ‘parking lot’ and two, the XY speed is 2X the speed of the Z axis, forcing the XY to slow down while the Z axis tries to keep up. Depending on the type of relief you are cutting and the amount of detail, here are a few speed combinations I have found to work, without symptoms of the tool slowing down to wait for the Z axis: 2,1 – 2,2 – 3,2 – 3,3 – 5,3. Unless you are cutting very large or long 3D parts, you probably won’t get over about 5 IPS. 3D cutting is very different from 2D cutting since the tool has to fight gravity and push and pull a gyroscope (your router) into your work at a high rate of speed. If you make sensible decisions about your move speed and adjust [VR] by observing the movement, sound and smoothness of your tool, you can transform your CNC to match the type of work that you do.

Saving Your Specialized Settings to Use at Another Time

OK, so you have your [VR] settings dialed in for perfect 2D cuts. You can type in the US command and save your configuration with a meaningful name, like ‘Brady2D.sbc’ and then move on to tune your tool for the type of 3D cutting that you do. You might want to save a configuration for V-carving and another for 3D relief cutting as well. After you have saved each configuration, you can easily call it up by typing in the UR command. It will ask you if you want to reset the current configuration. After affirming that this is what you want to do, you will see a list of configurations that you can choose to load, including the ones that you saved from your tuning sessions.

My next report ... under wraps.

The BradyVac II – A Production Vacuum Fixture on a Shoestring Budget - July 2007

About 2 years ago, I set out to create a removable universal vacuum fixture for doing various jobs. (Please review my Nov. 2006 article) This universal fixture was coined the ‘BradyVac’ by Bill Young. The basic idea is to take a sheet of Trupan or other ‘bleeder’ material, machine a grid into it, flip it over and have an entire surface that would pull vacuum through the face of the sheet. This of course means that you must actually have a vacuum and a vacuum port - or hole - in your support board/spoilboard where the vacuum plugs in. All of the fixtures and solutions I have created are used in conjunction with a single Fein Turbo III vacuum, which is designed for industrial use. You can buy the Fein Turbo III directly from ShopBot for $399. I have run my Fein at times for 25+ hrs straight and it is a great unit for any shop. Keep in mind that the BradyVac and BradyVac II can be used with any vacuum source, from a single Fein vac to a full tilt roots blower and everything in between. It is important to note that you must have free-flowing vacuum air going to the underside of the BradyVac sheet in order to get the full advantage of this configuration. It is not meant to be used with a dedicated bleeder board since this restricts vacuum flow. Only you can decide what vacuum system will serve the needs of your shop, and in many cases a single Fein is not adequate for certain types of production. ShopBot sales and support staff can help you determine the most appropriate vacuum setup for your needs, if you need some additional guidance.

The subject of vacuum fixturing is a hot topic, and many are confused by how vacuum can be used as a production aide when cutting various types of parts. While vacuum is not the solution for all sizes and shapes of parts, it is often a viable alternative to screws, clamps and tape when you have a stack of sheets or boards to cut for a particular job. The original BradyVac is geared towards those who want a universal solution where they may be cutting one size part now and then a different sized part later. You can make the BradyVac any size you choose as long as you have a vacuum port in your table to feed vacuum to it. This works pretty well for many parts, but there is a trade-off when using a bleeder board. You get the advantage of reduced vacuum pressure loss when you cut all the way through your part. The cutting tool creates a kerf where vacuum will escape from the bleeder, but at a much lower rate than an open-air setup. This is why pegboard works great until your tool cuts all the way through the part and leaks out the vacuum. The bleeder functions to slow down the rate of vacuum loss, but it comes at the price of not being able to fully exploit all the vacuum power you have at your disposal.

Purpose-built vacuum fixtures that directly expose the bottom of your parts to vacuum have superior holding power. These types of fixtures are suitable for solid wood planks, small parts and rapid machining where your feed rates are fast and material cycle time needs to be kept in step with a production schedule. Some purpose-built fixtures require gasketing to make the best use of vacuum, and to provide traction when parts have a tendency to rotate into the bit at the last second of cutting. Many fixtures benefit from the gasket materials offered by All*Star Adhesive Products. Check out their website to learn more about these products, and see the example at the end of this article. While fixtures of this type are very effective, the amount of time and cost in constructing this type of solution is often prohibitive, depending on the scope of the job. If the customer will consistently re-order the exact same parts from you over the life of the fixture, then this cost can be amortized over several production runs. Since creating vacuum fixtures costs you in time and materials, you should charge the customer for them or build this expense into the cost of the job.

Better, Cheaper, Faster…

If you are anything like me, you invariably have some jobs that need to be quickly and effectively machined in the shop in order to satisfy the customer’s deadline. Taking the time to engineer a custom vacuum fixture is often viewed as a gamble. Will it work? How long is it going to take to make? What’s it going to really cost me? Whether or not it will work is a question that I cannot answer without knowing what vacuum you are using, the size of your parts and other factors. I always encourage users to do their own R&D to determine through experimentation the realistic limitations of their vacuum power plant and method of delivering vacuum to the part. The real key with vacuum is efficiency. By this I mean understanding the limitations of your vacuum’s suction (inches of mercury) and flow rate (CFM), and how get the most out of it. The majority of my experiments have used a single Fein Turbo III, which to date has successfully held down parts ranging from 5/8” square to full sheets with no skin or tabs left on the bottom of the parts. In some cases gasketing was used to reduce leakage and part movement. Only through your research will you really know what your system is capable of and how to best leverage its ability. The goal of all of the BradyVac configurations is to cut all the way through your parts with no bridges/tabs in the fastest most efficient manner possible, yielding parts with superior edge quality. When configured properly and sensibly, vacuum will prevent vibration and material movement that can influence cut quality. Better hold down means better looking parts. Aside from software preparation, holding your parts to the table is the entire job in CNC. Everything else is relatively easy to accomplish.

A typical 4x8 BradyVac II takes about 1.5 hrs to make. It takes about 30 minutes to create toolpaths needed for the grid on the bottom part of the sheet, plus part boundaries and vacuum channels on the top part of the sheet. It takes about 30 minutes per side to machine the grid and the in-board plenums that sit under each finished part. It may take you more or less time to make your fixture depending on your skills & feed rates. The BradyVac II goes one step further than the original BradyVac by using your part vector outlines as a basis for creating the fixture so that everything lines up with your master cutting file. You can think of this system as a collection of individual vacuum pods that are adhered by the BradyVac sheet itself.

In terms of cost, if you want to really get the most out of this system, you will need a sheet of Trupan Ultralight MDF. It consistently bleeds vacuum through its face compared to regular MDF, which has been known to have varying resin content. This resin content effectively seals off the porosity in the middle layers of the sheet and will not work with the original BradyVac. However, any material can be used with the BradyVac II since vacuum will flow through the grid and into individual plenum areas under each part. The only disadvantage of not using Trupan with the BradyVac II fixture is that your scrap material will not be held down by vacuum pulling through the face of the Trupan. If you use a non-porous material to construct a fixture, you will want to add some additional plenum areas to hold your scrap in place while cutting. Many overlook this important step since scrap can get stuck on your dust collector, tooling or other moving parts, potentially becoming a safety hazard.

Let’s take a look at the basic anatomy of the original BradyVac first and then the BradyVac II so that you can get a complete understanding of how it works.

The foundation for the BradyVac I or II is a sheet of Trupan with a grid machined into it and flipped over with the smooth un-machined face pointing up. The only other thing you will want to do is edge-band or seal the edges of the sheet since a substantial amount of vacuum can be lost through the edges of the sheet. The edges of a ¾” sheet of Trupan equal just over one square foot of area that will leak vacuum if left unsealed. You can use edgebanding, foil, painter’s or duct tape to seal the edges.

Bill Young created a BradyVac virtual tool in the ShopBot Labs area of the site for those that want an easy way to create vacuum grids. You can check it out HERE.

The examples above show how your vectors need to be setup for machining the BradyVac II. You will need to create four toolpaths to machine your fixture. First, use your part vectors and offset them to the inside of your part about .125” to .25” to create an Area Clear/Pocketing toolpath about .125” deep. This will serve as a mini plenum that will direct vacuum air only under the parts you want to cut. Note that if your material is thin or flexible, you’ll want to put some ‘islands’ in the middle of the Area Clear to keep the material from flexing downwards towards the plenum. Then create some .5" to .75" diameter circles where you know the tool will never cut. Use them to create an Area Clear .125” deep. These will become countersunk screw holes to fasten the fixture to your spoilboard so that it doesn’t move when you swap out sheets. Then create a Machine Along Vector toolpath about .3” to .4” deep, to puncture through to the grid below. You want this to be deep enough to intersect the grid channels below. Make the Machine Along Vector lines perforated to keep some strength in the grid. Finally, use the same vectors to run a 90° V-bit into the channel to clean up the channel and increase airflow. Place your material on the fixture and start cutting!

This setup certainly brings a lot of versatility to your machine with even the tightest of budgets. A typical BradyVac II can be built for under $30 using Trupan Ultralight. I have personally cut over 10,000 parts using this type of fixturing on parts of various sizes. The fixture works so well that I was able to increase my cutting speed from 2.5ips on one project using the original universal BradyVac to 7ips using the BradyVac II. Your results may vary, so be sure to conduct your own research using your tool and vacuum system.

A couple tips for production

Be sure to ‘crown’ your material before placing it on the vacuum fixture. If the material has any type of bow to it, you’ll want to have this pointing up towards the ceiling. In this configuration the vacuum can pull it down flat. If the material sits on the table like a potato chip, the vacuum will have a difficult time sealing, unless you flip it over. Severely bowed lumber may not be suitable for vacuum fixturing without the proper gasketing. You should plane or prepare solid wood before attempting to hold it down with vacuum if it is bowed, twisted, rough or otherwise disfigured.

When using the BradyVac II you will get some chips & swarf in the channels of the vacuum when you remove your parts and scrap. You want to take care not to disturb the raised vacuum seal between your cutting tool tracks and the center area clear/plenum. A vacuum wand can easily damage this and cause leakage. There are two ways I have found to clean off the fixture for the next sheet. 1) Blow off fixture with compressed air. 2) Program the CNC to drive around the sheet picking up the bulk of the debris with the dust collector and then blow off the small remainder. No dust collector is going to get all of the chips off due to static cling or chips getting embedded into the fixture because of vacuum suction.

Additional Examples

You can also use gasketing in many different configurations using the BradyVac system. It is  more efficient to drill holes through to the grid then attempt to cut the gasketing with a router bit, as it tends to tear the gasketing rather than cut it cleanly, even using a special bit recommended by All*Star with a climb mill strategy.

&

In a future article, I will be showing you how to create economical vacuum pods using off the shelf material. These are perfect for long moldings and other long, thin parts.

A Tale of Three Bits…and The Poor Man’s Compression Spiral Trick - March 2007

Selecting the right bit for cutting sheet goods can be tricky, so we’ll shed some light on different bit geometries you are likely to encounter and when to use them. For most sheet goods, a regular 2-flute straight bit is a good choice. It neither pushes nor pulls the chips up or down, and it neither helps nor hinders your hold down method. The downside of 2-flute straight cutters is that they don’t have the same strength as their spiral counterparts, especially in ¼” or smaller diameters. I have yet to find a ¼” 2-flute straight bit that will last long before breaking, even with a very light chip load. If you examine a small 2-flute straight ¼” bit you will quickly see how small the center cross section is compared to a spiral.

When it comes to spirals, there are generally 3 different classifications, as they relate to cutting sheet goods.

1. The Upcut Spiral – This does an excellent job of evacuating chips from the kerf, pulling away heat from the bit. The upcut action of the bit leaves a smooth bottom face on your sheet goods and reduces the chances of burning and melting of materials. The downside of using an upcut spiral is that it can fight your hold down method and lift parts when cutting thin materials. The other downside is that it will often chip out the top veneers on sheet goods, resulting in a less than desirable finish. Upcut spirals are typically the same grind as a standard solid carbide end mill used in the metalworking industry. You can save a considerable amount of money using end mills instead of upcut spiral router bits.

Notice how the flutes of an upcut lean toward the right, when bit is viewed vertically as it would be in the router. This is also called a right-hand spiral cutter. By holding the cutter by the shank and rotating clockwise, you can simulate the rotation of your router and understand how the flutes lift the chips out of the kerf with an upward action.

2. The Downcut Spiral – This does the exact opposite of an upcut spiral. It pushes chips back into the kerf and can sometimes blow out the bottom face veneers when it cuts all the way through. Since it forces chips back into the cut, it is prone to burning and melting and welding chips to materials. A downcut assists your hold down method and is ideally suited to shallow cutting and thin materials that would have a tendency to lift during cutting. It does an excellent job on top face veneers virtually eliminating tear out.

Notice how the flutes of a downcut lean toward the left, when bit is viewed vertically as it would be in the router. This is also called a left-hand spiral cutter. By holding the cutter by the shank and rotating clockwise, you can simulate the rotation of your router and understand how the flutes push the chips and material with a downward action.

3. The Compression Spiral - This is a combination of an upcut and downcut spiral. When run in a single pass it gives a relatively neutral cutting action, mildly assisting your hold down method. To get the full benefits of a compression spiral, it is meant to be run full depth in the material, cutting the sheet in one single pass. Compression spirals run in multiple stepdown toolpaths show the same detrimental qualities of the upcut spiral, having a tendency to tear out the top face veneers. The reason it will do this is in the geometry of the bit. Typically, compression spirals have an upcutting single flute at the tip of the cutter approximately one third of the cutting length of the bit. The remaining two thirds is ground to give a downcutting shear. When run full depth, the bit leaves a sharp clean top and bottom face. When a compression bit is run in multiple passes, the 1st third of the bit, being an upcut grind, pulls the face veneers out and users are left scratching their heads. Compression bits work best when ramped into a cut in the XZ or YZ plane. This is typically an option only found in some of the more advanced CAM packages, so it is not something that you can do with only PartWizard…but now I am going to show you how to get the same quality cut of a compression spiral using PartWizard. (See additional information at the end of this article concerning compression spirals.)

Notice how the compression spiral is a combination of an upcut & downcut grind tool. Approximately 1/3 of it’s cutting length is upcutting, the remainder is downcutting.

The Poor Man’s Compression Trick

This is a technique that I coined as a ‘poor man’s compression spiral’. It actually uses 2 bits: A downcut and an upcut, plus two toolpaths. It requires a bit change in between files, but if cut quality is your highest concern, this is well worth the added effort.

I’ve created a file in PW3 for cutting out some sheet goods in .75” thick material. I created two toolpaths, one with a downcut spiral bit to break through the top veneer of the material to give me a nice clean top face. I have limited the depth to .25” and I have set the stepdown to .25” so that it will do this in a single pass:

Examine the toolpath assistant on the left and notice how the depth is restricted to .25” deep. I named this toolpath DownCut_1 so that I would remember that I am going to run this toolpath first using a downcut bit.

Next, I left the toolpath assistant open and changed the start depth from 0 to .25”. Remember, our downcut is already going to cut down to .25” deep, so there is no sense cutting air for the 1st pass. I then changed the finish depth to be the thickness of our material, in this case, .75”.

I named the toolpath UpCut_2, since it will be cut after the toolpath we created previously. It will start at .25” deep, and do two passes, one at .5” deep and the final pass at .75” deep. Since it is an upcut it will pull the chips upward and leave us with a nice clean face on the bottom of our material. Using this method, you get all of the benefits of a compression spiral using common bits available at any home center or lumber yard. The inconvenience of a tool change is quickly overshadowed by the quality of the parts coming off of the machine, and the fact that your average compression spiral bit is in the neighborhood of $65 or more. The poor man’s trick can be done with about $35 in bits if you shop around!

Compression Spirals – Things to consider:

The idea of using a compression spiral is appealing, but there are some additional things to consider when using these tools. Your ShopBot is equipped to deliver between 70 and 150 pounds of cutting force, depending on the model. Cutting full-depth in .75” material places additional load on the tool, and some fine tuning on your part is needed to make sure that you are cutting first class parts. While it is important to consider chip load when calculating cutting speeds and RPM, it is equally important to consider the column of material that is to be evacuated by the cutter, and the force that is going to be applied to the material. Physics 101 taught us that for every force, there is an opposite and equal force applied. This means that if you are using vacuum to hold down your parts, you need to consider how effective it will be against the force of the cutter. You will also need to consider bit deflection and how that can influence the accuracy of your parts.

Those running PRT Standard tools, will want to avoid pushing the tool beyond what the stepper motors are capable of delivering since they lack positional feedback. Loss of steps (where magnetic lock on motor is temporarily broken) will result in off-spec parts, when you ask the motors to do more work than they are designed to provide. Those using Alpha-spec tools should understand that even with positional feedback, you can run the tool too fast, and trigger ‘Alpha mode’ where the tool self corrects momentarily causing a small deviation from the programmed cutting path. If you are losing steps (standard ShopBots) or your tool is going into Alpha mode, you will need to reduce the cutting speeds, and adjust the ramping values (VR) for your tool. Adjusting your ramping values will greatly enhance the performance and flexibility of your CNC regardless of what tool or material is used.

There is also another thing to consider when running compression spirals. There are many professionals running compression spirals with their ShopBot day in and day out, cutting thousands of sheets a week. The added force required to run these tools places additional stress on the rack and pinion drive system. If you plan on processing sheets on a daily basis using compression spirals or any high-speed machining operation, a close examination of your pinions is a must. Pinions are consumables, wearing many times more quickly than your rack. Make inspecting and replacing worn pinions part of your ShopBot maintenance schedule to ensure that you continue cutting smoothly and on spec. New pinions are inexpensive enough for even the smallest shop to build into their maintenance schedule.

A Removable Vacuum Plenum that Maximizes Hold Down Potential - November 2006

If you are anything like me, you want to be ready for any job that comes through the door. For me, this meant being able to quickly tool up for cutting 2” hardwood shapes that needed to be screwed down to a rigid spoilboard one day, and be able to hold down 4X8 sheets using vacuum the next. One method would be to turn the vacuum on and pull down the bleeder board so that I could screw into it. I wasn’t keen on running the vacuum all the time since it seemed like a waste of energy.

I got a call from a customer who needed me to cut 32 intricate grill shapes in ¼” PVC over night in order to meet their deadline. The material blanks were already pre-cut and all I needed to do was hold them down. The thought of carpet taping all of the parts down was not very appealing to me, so I decided to try making a combination bleeder/vacuum grid from a single piece of Trupan. I’ve been very successful using interchangeable vacuum ‘masks’ for holding miniature parts before with a bolt down plenum. The use of AllStar Spoilboard Cover gasketing really makes a difference when holding small parts.

I began by making up a simple grid in PartWizard using a Machine Along Vector Strategy. I cut the grid into a piece of 18mm Trupan Ultralight MDF .25” deep using a ½” bit, then cut it out of the sheet. I then cut a 2.27” hole in my spoilboard to accept my Fein Turbo III’s 2.25” vac hose with a .02” allowance to make sure that it fit. I plugged in the vac and put the Trupan over it with the grid side down. I then used the CR command to flatten it just like I do my spoilboard. This breaks the paper barrier on the outside and exposes the porous matrix of the Trupan. I then added some AllStar 1/32” gasket tape to the bottom perimeter and did a once around with some duct tape to seal off the edges of the Trupan. I wanted all the vacuum that I could get!

In order to be successful with vacuum you want as much surface area of your parts exposed to the vacuum, but not so much that you create a leak and sacrifice holding power. If I were to place the material blanks on the combo board with no ‘mask’ it would hold for a few minutes while cutting until enough of the bleeder board had been exposed to the atmosphere. Then the parts would move and be ruined. To avoid this, I created a vacuum mask out of 1/8” acrylic that I had laying around the shop.

I started with the vectors I was going to use for the profile passes and offset all of them .03” inside. This is a good place to start to keep the vacuum from leaking out of the kerf when cutting. I then did a block copy of 1/8” holes as large as my part. I deleted all of the holes outside of the offset boundary that I created. These holes expose the part we want to keep to the vacuum and direct all of the vacuum’s resources to holding our part. After drilling all of the holes, I placed the acrylic mask on top of the Trupan bleeder and placed my material blank on top. Be sure to use the same file for creating your mask, as you do for creating the profile passes. This way everything matches up when it comes time to cut.

The gamble paid off! It really worked! In fact, this worked so well that I decided to make a full 4X8’ version that I still use today. I tack the big one in with brads and make sure that I have a good seal around the edge. A single Fein holds down a full sheet of plywood, letting me cut parts all the way through. It isn’t a 15HP professional setup, but when the day is over and I have to screw down heavy parts, I can simply pry it up and re-use it the next time I need it.

The Keys to Success - May 2006

During the 2006 ShopBot Jamboree I demonstrated how you can substantially increase your drawing efficiency and effectiveness by using the built-in short cut keys in your design software. In many cases, the short cuts allow you to do things that cannot be done using just the icons and menus in PartWizard, Insignia and ArtCAM Pro. In the picture below, you can see the short cut for ‘Copy’ highlighted next to the menu item.

In this case and many others, you can use standard Windows short cut keys to do the same function within the program. For example, you can use Ctrl + X to cut selected vectors from the model and store them on the Windows clipboard. As long as you don’t Copy or Cut any other vectors, they will remain there. To bring them back, just us Ctrl + V to Paste them back in. An interesting trick that takes advantage of these short cuts is to open another instance of PartWizard and Copy & Paste vectors from one screen to another. This effectively gives you multiple layers just like Insignia and Pro. This is particularly helpful when doing complex designs that need a buffer area or layer to store vectors until you are ready to use them again.

Download the following list of short cuts and try them out for yourself.

Download Short Cuts (pdf quick reference sheet; click here)

Be sure to check out some of the secret short cuts that I discovered in PartWizard, such as the ability to join multiple vectors:

If you take the time to use and commit to memory the commonly used short cuts & use them when you draw, you will be able to do more in less time. Remember, the best way to learn the software is to play, play, play! So fire up that computer and draw something that is not work related. This way, when you do something for a customer, you will remember what you did when you weren’t under pressure during one of your play sessions. Try it!

A Sticky Situation … - March, 2006

Sooner or later every CNC operator will come face to face with a challenging material hold-down problem that cannot be solved using conventional methods. Clamps get in the way, tabs/bridges require post-finishing of the part, screws don’t hold the part down in the center and vacuum is sometimes not strong enough for small parts without specialized gasketing.

One very versatile and effective method is to use carpet tape. There are a few different configurations of carpet tape out there. You want the stuff that has coarse fiberglass mesh in it that is labeled ‘Indoor/Outdoor’. There is adhesive on both sides of the mesh and the adhesive is protected by a paper coating until you are ready to remove it and secure your material. When you are ready to secure your material to the spoilboard, clean both the spoilboard and material to be secured. Apply carpet tape to the spoilboard if you are cutting a full sheet, or to the part for smaller material. Then, run a laminate roller down the tape to get good adhesion. Remove the paper being careful not to kick up any dust or debris. If you are handling a full 4X8 sheet, have someone help you place the sheet squarely on the spoilboard. If you don’t place it carefully and move it, the tape may get displaced creating a lump of tape under the material. After you have placed your material on the adhesive, press down or walk on the material to create a good bond. You are now ready to cut with no tabs, screws or clamps.

Depending on what you are cutting, you will want to use discretion when deciding just how much tape is needed to hold a part down. Not enough will cause a part to move when being cut and too much…well, let’s just say that you will have a really tough time removing it from the spoilboard! Experiment a little to find out what is best for your application. In some cases, the tape will leave a residue on your finished parts. You can remove it with either denatured alcohol or acetone. Always test a piece of scrap before using solvent on your finished pieces to determine if it is compatible! Acetone is not compatible with most plastics and will either de-gloss the surface (e.g. Sintra or Komatex) or melt the surface (e.g. acrylics & others). In most cases denatured alcohol will not harm your parts, but it takes a bit more rubbing to remove it from the part compared to acetone. Using denatured in a spray bottle & keeping the part wet while rubbing does the trick.

One thing that is nice about carpet tape is that it is available pretty much everywhere. I usually buy the Indoor/Outdoor or High-Traffic labeled Duck brand at Home Depot or Lowes. It comes in a few different widths and lengths. I buy the 2.5” X 75’ rolls for about $8. When I don’t feel like going all the way to Lowes or Depot, I go to my local Ace Hardware. They also sell the Indoor/Outdoor Ace-brand version in 42’ lengths. They sell a 1.5” and 3” version. Get the 1.5” version as the 3”, for some unknown reason, tends to not release from the protective paper. You may also want to experiment with upholstery tape, but it lacks the fiberglass mesh that helps you to pull the tape off in one shot.

For those who have the ShopBot digitizing probe, you will find carpet tape an excellent solution for holding part securely to the spoilboard for digitizing. This allows you to hold down parts that cannot be screwed down, clamped or damaged! This method is applicable to both 2D and 3D digitizing. Give it a try, I’m sure that you will find it a great addition to your current hold-down techniques!

Just a Little Bit ? - January, 2006

If I had to describe my ShopBot CNC in one word, it would be, ‘versatile’. I can’t think of any other tool that I have purchased during my lifetime that can do as many tasks that my ShopBot can. I think that ShopBotters are also equally versatile, especially when it comes to doing big things on a small budget or inventing new economical solutions to seemingly expensive problems.

One really great aspect of a ShopBot tool, is that you can add accessories and customize your machine as your budget allows. This means that if you can’t initially afford a spindle, you can still get started right away with a standard woodworking router as your cutting tool. (Spindles typically run smoother and quieter than your average garden variety wood router. They have precise speed control, higher duty cycles and offer collet sizes that can accommodate bits from 1/16” to 5/8” diameter, typically in 1/16” increments.)

But I know that many ShopBot owners who have a standard wood router on their ShopBot, want to try their hand at engraving, or take advantage of 1/8” shank tools for finer work. The problem is that most router manufacturers don’t make accessory collets for their tools outside the normal ¼” & ½” sizes. The first thing that I tried was one of those collet-sleeve adapters; you know, the kind with the ¼” shank and set screw? It was hardly worth the effort because the run-out caused by the poor fit of the 1/8” bit made precise cutting impossible. That’s where the story ends for most of us stuck with ¼” & ½” collets.

Well I’ve got some good news for all of us with a standard router! While browsing for metalworking tools, I stumbled across a ½” shank ER-11 “Stubby Collet Chuck”. The ER-11 chuck slips into any ½” collet like any other tool, but has a miniature collet & nut on the tip of it. It has an overall length of 3.5” and it only costs $65. For about $15 apiece, you can get collets that accept 1/32, 1/16, 3/32, 1/8, 3/16, 7/32 & ¼” shank tools. This means that you can use cheap end mills and specialty bits in your standard wood router! To add to this new-found flexibility, you can buy the ETM-brand collets, which give you a collet range of .04” +/- advertised diameter to fit those odd-sized or even metric shank bits in your router. The collets & holder are designed for high-precision and have an advertised run-out of only .0002”; which is a lot better than the set screw insert I initially tried. ER-11 stubby collet chucks are available from many of the larger industrial supply houses. Be sure to get a set of ER-11 wrenches so you can use your small bits as soon as the collet chuck arrives!
 

Here's a link to Enco, who sells the collet holder & ER11 collets: www.use-enco.com
  [Enco Part Numbers: Stubby Collet Chuck: Model #308-0018, 1/8" ER11 ETM Brand Spring Collet: Model #891-6984]