Equipment and Software Assumptions
Ø 3-Axis CNC Plasma Table, Assembled and Operational
Ø Fully Functional Z-Axis With Floating Head (pic - Z_Axis.jpg)
Ø THC-300 (Torch Height Control) Hardware, Installed (http://www.campbelldesigns.com/)
Ø SheetCAM CAM Software, Must Be Familiar With the Basics (http://www.sheetcam.com/)
Ø Mach2 v-6.11b, Windows/PC Based CNC Controller Software (http://www.artofcnc.ca/)
Ø Willing to Get Exited About Consistently Achieving Successful Cuts!
The purpose of this tutorial is to provide a direct path for new users to get their CNC plasma machines up and running with the least amount of pain. This is not a comprehensive manual by any stretch of the imagination and once you’ve accomplished good cutting techniques, all further honing of your skills will come with the help of user groups, manuals, and most definitely hands on experience.
The following content assumes the user has previously installed and possesses a ‘basic’ understanding of how the various features and controls of SheetCAM, Mach2, and THC-300 operate relative to their contraption. Please keep in mind that the configuration settings found in the following pages are intended exclusively for Plasma users, flame cutting and the like were not considered when writing this guide.
Note: Screen captures and pictures are provided within this tutorial to assist you in setting up your machine. The filename of a screenshot or picture will be indicated as relative to the topic. i.e.: (pic/screenshot - samplepic.jpg).
Lets Start With Mach2
Mach2 is a very customizable CNC controller that can be used to control several types of CNC machines. For the purposes of this guide we will only be focusing on the features that pertain to plasma cutting. As you will soon recognize, the author of Mach2 generously integrated a few plasma specific features that help make plasma cutting and THC possible in this hobby oriented CNC industry that we find ourselves. Hats off to Art!
Configuration File: Otherwise known as the “Profile” file, the configuration file retains all of Mach2/s configuration settings, including the parallel port and pins mapping values. It is not within the scope of this tutorial to explain in any detail the values of breakout board specific connection parameters given the numerous techniques for connecting your electronics. With that said, if you purchased your breakout board from a reputable supplier, then chances are they will also provide either a configuration file or a list of settings that can be manually entered in Mach2.
Whether you purchased a breakout board along with your THC-300 from Campbell Designs or not, a file named THC.xml is provided with this guide that will accommodate you in the set up process. To make use of this file, simply place a copy of it in Mach2’s installation directory. If you selected Mach2’s default installation path during setup, then you can find this directory by browsing to C:\Mach2. Once the file is in Mach2’s directory it will automatically appear in the “Session Profiles” dialog upon clicking the ‘default’ Mach2 icon. At this point select THC300; press OK, and the correct settings will be automatically applied when Mach2 loads.
As a second option, you can omit the “Session Profiles” dialog and launch the THC300 settings directly when Mach2 loads. This can be accomplished by right clicking on the Mach2-Mill icon (or any other icon) and replace the “Target” property text with “C:\Mach2\Mach2.exe /p thc300” (that’s without the “ ” marks of course), and then clicking Apply/OK (screenshot - Icon Properties.jpg). You can now rename the icon to your liking, perhaps “Mach2 Plasma” or similar would be a good name for future reference.
If you are not using the breakout board from Campbell Designs, then you will now need to manually change the ports & pins settings that concern your particular hardware.
Screen File: Just as a configuration file exists for your settings, a Screen File also exists containing a set of Mach2 customized screens that was intended to be used with 1024/768 screen resolution. This file defines the components (buttons, DRO’s, etc.) within the various screens along with their location, size and appearance. A file is provided named THC300.set along with this guide containing a modified set of screens that were designed particularly to be conducive to plasma cutting. The main screen, or Run screen consists of controls and indicators that you will need quick access to during routine jobs. The other six screens provide various controls and data that allow you to configure and troubleshoot the machine when necessary. To make use of this file, place a copy of it the Mach2 directory. The configuration (THC.xml, mentioned above) file includes a reference to the THC300.set screen File, thus, commanding Mach2 to load these THC300.set ‘Plasma’ screens upon startup.
State Dialog: View (screenshot - State.jpg), here we will only need to change a couple of settings. Since we selected SheetCAM as our premier CAM software we will need to let Mach2 know how to interpret the g-code it generates. In Mach2, select the Config menu, then State. Within the “Initial State Settings” dialog box, set IJ mode to Inc. In the same dialog box, set the “Z” Reference Switch Loc (otherwise known as “Lost-Z”) Z-value to the ‘negative’ travel your Z-axis travels downward beyond the point it touches the material, just to the point it makes contact with the Z reference switch. The point of ‘switch contact’ can be observed in the “Diagnostics” screen of Mach2, be sure your polarity is correct (active state), meaning you should only see a signal for “Z-Home” when the switch is engaged.
Overview and example, my setting is -0.21 inches, this value represents the distance in inches (because I selected Inches as my preferred units in Mach2) my torch travels down from the material surface to the negative value in which it makes contact with the reference switch, taking into account that for the purposes of this test the material surface is equal to zero on the Z axis. This setting is extremely important and will affect each and every cut you make in the future, therefore, be absolutely certain this value is accurate.
Logic Dialog: View (screenshot - Logic.jpg), here we will only change one setting, but it will take some length to explain the reason it exist. In Mach2, select the Config menu, then Logic. In the “Logic Configuration” dialog box, notice the “Plasma Mode” check box. Depending on the mechanical ability of your machine, you may, or may not decide to check and enable the “Plasma Mode” feature.
Here’s the concept, while in Plasma Mode Mach2 will apply an algorithm in efforts to compensate for the characteristics of a plasma flame in some circumstances. When a plasma flame is active, or able to make electrical connection with its opposite polarity it will intensely be attracted to the material the cable clamp is attached to. Therefore, if the flame were held stationary, it would continue to erode (burn) away material for as long as it could remain active. In the case of CNC, it’s important to not stay in one place for too long while the flame is active; otherwise, the part being cut will reflect such erosion. The setting “Plasma Mode”, being selected or not, depends on your plasma machines capability/settings and the thickness and type of material being cut, it’s a question of material removal rate. At a high rate (typically higher current) your torch needs to move quickly at all times to prevent excess erosion, especially on sharp corners where most machines will most notably slow down. Some machines can perform at high rates throughout the cut; others can perform at high velocity rates, but cant accelerate/decelerate at high rates. With Mach2’s Plasma Mode feature the controller attempts to maximize the speed in the corners for the slower accelerating machines, which is based on your machines Motor Control settings that you enter. Mach2 then attempts to take out the remaining portion of slow corner speeds with a sort of ‘rounding off’ sharp corners effect. The intention isn’t to leave rounded corners; the flame will erode some material in the corners due to slight slow down, hence, leaving the corner relatively sharp. This feature is fair to describe as complex, maybe this is why Art, the author of Mach2 calls it a ‘proprietary’ algorithm. The long and short of it is, test your machine with and without Plasma Mode active on materials you regularly cut, and only then will you acquire a satisfactory decision on whether to use it or not depending on the quality of the finished part and the smooth traverse of your machine.
THC-300 Controls: The controls that were added to the Mach2 screens for THC can be found on Mach2’s main screen under the label “Torch Height Control”.
The minimum and maximum distance Mach2 will command your Z-axis to correct for varying torch height can be set under the label “Maximum Correction”. These two values should be set within the limits of what can be reasonably expected of the THC-300 to correct height based on the condition of the material being cut and the physical travel capability of your Z-axis. My machine is set at max = 3”, and min = -.15. Keep in mind that if Mach2 is commanded to travel beyond these parameters motion will continue, I don’t know why, but it does, so be especially critical for the lowest setting to prevent a collision with the torch.
The “Z-Speed %” tells Mach2 how fast to correct an up or down signal received from the THC-300, this rate adjustment is relative to the Z-axis rapid feed rate. For example, if your maximum feed rate for the Z-axis is 100 (inches or millimeters, based on your settings), then a value of 20% in the “Z-Speed %” box will command the Z-axis to correct any height changes at a rate of 20 upon receiving a signal from the THC-300 to do so. A ‘too high’ of a setting will cause the Z to overshoot, and a ‘too low’ setting will cause the Z to not respond quickly enough to the varying height of the material being cut. Only experience will give you the proper settings for this parameter based your machine and the flatness of the material being cut.
The “Enable THC” toggle button is self explanatory, when enabled, the indicator to the right of it will illuminate green, and when disabled it will appear grey.
The “Anti Dive” toggle button is similar in function to the Enable THC button in terms of color response of the indicator. A description follows as to its functionality below.
The “Auto Dive Limit”, when enabled by selecting the “Anti Dive” toggle above and with the indicator thereof illuminated green, is the Rate limit of the X or Y-axis that Mach2 stops responding to height signals from THC-300. In other words, if, and when either the Y or X-axis rate falls below this value, Mach2 will halt Z-axis output in response to THC-300. This feature is designed to prevent false height feedback from THC-300, which can happen if the X/Y traverse rates are reduced significantly. Perhaps because of the inability of your machine to maintain high speeds because of the need to decelerate, then accelerate in and out of sharp corners. When this slowing occurs, THC-300 will naturally detect an increase in arc voltage and will falsely signal Mach2 to lower your torch. This parameter is dictated by your machines abilities and the content of the g-code/feed rates commanding it. Therefore, experience is the only way to decide whether to use it or not, and if so, what setting works best for a particular job. It’s not required on my machine.
The label “Current Correction” DRO (digital read out) is a read only data box that shows the ‘current’ height correction applied to the Z-axis.
The label “Arc Good’s” indicator illuminates green after the THC-300 informs Mach2 that the plasma machine has signaled the arc becomes successful following a pierce. The arc good signal can be lost during a cut if for whatever reason the torch cannot maintain an arc. Perhaps the most common reason is when the torch runs off the end of the material or runs over an existing hole etc.
The label “Dwell Active’s” indicator illuminates green when Mach2 is commanded to delay, which usually occurs when the “Pierce delay” set in SheetCAM is timing out.
The Mach2 settings above assume you took advantage of the settings provided in the THC300.xml file. If a setting was not mentioned, then it should remain as it was set in the original THC300.xml file. If you decided not to make use of this file directly, then open it with an Internet browser and transfer all other settings unrelated to your specific hardware to Mach2 manually.
SheetCAM is a CAM (computer aided manufacturing) program designed to take the conjecture out of generating g-code, not to mention the time savings it provides even for the g-code writing guru’s. There are many CAM programs on the market today, but SheetCAM currently competes unmatched with respect to ease of use, features, and support vs. cost.
Post Processor: A post processor is a text file that contains programming code that SheetCAM utilizes as its guiding light. SheetCAM refers to the code in the post processor for any machine specific functions, thus, allowing SheetCAM to be a universal 2-1/2D g-code generator. For our purposes, SheetCAM’s post processor can be modified to control virtually any plasma table. There is a post processor file provided named PlasmaTHC300.post with this guide that was designed to work with the type of Plasma machine described in the “Equipment and Software Assumptions” section above. This post processor allows SheetCAM to make all of the command decisions concerning the motion of your machine, including pierce height, pierce delay, cut height, pause at end of cut, and so on. It also includes a conservative method for referencing the Z-axis at the start of every cut, other methods are available, however, it is recommend you use this post until you are comfortable with the process. To make use of this file, place a copy of it in SheetCAM’s subdirectory named “Posts”, next, open SheetCAM and select “Options”, “Select post processor” and browse to the Posts directory and select PlasmaTHC300.post, then click Open. SheetCAM now knows what post processor to use for your machine in which it will retain until you change it!
Tool/s: Plasma users of SheetCAM you can create several tools, one for each type of nozzle, or different types and thicknesses of materials being cut. Since I don’t use my machine in heavy production, I chose to simply create one tool and modify it per job. A screenshot (screenshot - Plasma Tool Options.jpg) of my tool settings dialog is provided with this guide. It was configured for cutting 3/8” thick mild steel plate with a Hypertherm Powermax-1000 plasma cutter, T60M mechanized torch, and using 60-amp shielded consumables.
The “Ramp lead in” feature found in your tool settings box will ramp the torch ‘starting’ at the pierce height and ‘ending’ at the end of the lead in, or cut height. This feature is designed to prevent the torch tip from diving directly in to the spatter built up while piercing, especially notable with thicker materials. Consideration should be given when setting lead-in lengths; unnecessarily long lead-ins may cause premature nozzle wear along with other unforeseen, adverse affects of holding the torch higher above recommended cut heights for long periods of time.
Units: You will need to let SheetCAM know what your preferred units will be, Inches or Metric. Select “Options” then “Units”, the ‘Units setup’ box should appear, select your preferences and click OK.
Now that you have selected your units, SheetCAM will use these selections as defaults and is what allows you to enter numbers without a unit description, like ‘20’ without the inches/min or mm/min etc. Otherwise, SheetCAM is smart enough to interpret values when unit descriptions are entered. For example, if you selected mm/in as your Feed Rate units, you can still enter ‘20 inches/min’ and vise versa for the Plasma Tool Plunge Rate. The descriptions tell SheetCAM your intentions and SheetCAM will automatically convert the entered value to that of your preferred units. The results, in the example 20 inches/min, will become 508 mm/min and will be displayed once you either press enter or click anywhere outside of the entry box. This feature is especially useful for entering recommended values found in the Plasma cutters manual that are different than your preferred units.
Note: For this feature to work properly you will need to use one of the unit descriptions found in the drop down list (inches/min, NOT in/min) of the “Units setup” dialog, else, SheetCAM will use default units for the numeric portion of any unrecognized entries.
Processes: When creating processes for your drawings there a couple of things to consider. First, if your drawings consist of a single layer, SheetCAM will work out which vectors (shapes & lines) to cut first, next, and so on. SheetCAM will cut the closest ‘open’ vector (line with non-connecting ends) to the start point first, then the next closest open vector until all open vectors are cut. Then it will cut the closest inner ‘closed’ vector (line with connecting ends) and so on until all inner vectors are cut. Finally, SheetCAM will cut the outer vector according to the offset settings you selected in the “Edit plasma cut” process dialog. All open vectors will be cut with no offset, all inner closed vectors will be cut with opposite offsets of that set in the Edit plasma process dialog, unless “no offset” was selected. The outer vector will be cut with whatever is set in the ‘Edit plasma cut’ dialog. If your drawing is broken up into multiple layers or if you organized your vectors on different layers in SheetCAM (see below), then its up to you to control the order in which each layer is cut. The cut order is the same order in which each process appears in the process list, most upper being first. To change the order, drag each process (with your mouse) within the list to match the order you would like them cut. Drawings divided into layers gives you complete control over lead-in lengths, offsets, and all other process parameters on a per layer basis. Multiple layers can solve problems such as applying different lead-in lengths for different shapes/vectors, cut order, and allows the ability to add g-code snippets between cuts.
A file named (screenshot - Processes.jpg) is provided with this guide and is a screenshot of SheetCAM with typical processes created using a two-layered drawing. It is organized with the inside vectors placed on a layer named “FIRST_CUTS” and the outside vector on layer named “SECOND_CUTS”. The “FIRST_CUTS” process dialog is open to show typical settings for plasma cutting.
Contour Properties: Once a drawing is loaded, you can reorganize its vectors with the contour control. SheetCAM refers to vectors as contours. Select the “Edit contour properties” button (one with a C) and the mouse arrow should now have a C next to it. Select any and all vectors you wish to place on a single layer by holding the Control (Ctrl) key down and selecting each vector. Next, right click over the drawing and select “Move to layer”, you can now either create a new layer or place the selected vectors on an existing layer within the list. Simply repeat this process until all vectors reside on layers of your choosing. Independent processes can now be created for each layer.
The THC-300 comes with a fairly concise set-up guide, therefore, a copy of it is provided with this guide named THC-300 Guide.pdf. Once the instructions in the guide are followed along with the instructions provided above, you more that likely will be able to operate the THC-300 without incident. Perhaps the greatest thing of significance when setting up the THC-300 is making sure the input signals sent to Mach2 are received as expected and with the correct polarity. You can observe this on the diagnostics page in Mach2.