CNC Plasma Cutter User Guide

From vector-space.org
Revision as of 11:45, 24 April 2021 by Kbogacik (talk | contribs) (→‎TROUBLESHOOTING)
(diff) ← Older revision | Latest revision (diff) | Newer revision → (diff)
Jump to navigation Jump to search

Shop Area: Metal Shop

Tool: CNC Plasma Cutter

Requires in-person training: Yes 

Procedure Number

UG 130-05, Rev. 1

Date

2/8/2021

 

GENERAL

This page describes the Langmuir Crossfire CNC Plasma Table. This is a 2 foot square table equipped with the 45 Amp Razorweld plasma cutter. It can be used to cut various sheet metals up to 1/2" thick.

CNC Plasma Cutter.png

SAFETY

  • Always wear approved safety glasses or face shield while operating the equipment.
  • The plasma cutter requires at least shade #5 eye protection. Welding helmets can also be used.
  • Before operating equipment, remove tie, rings, watches and other jewelry, and roll sleeves up past the elbows. Remove all loose clothing and confine long hair.
  • Non-slip footwear or anti-skid floor strips are recommended.
  • Closed toe shoes are required when working in a shop area.
  • Do not wear gloves while operating the equipment.
  • Make all machine adjustments or maintenance with the machine unplugged from the power source.
  • Never cut or weld material with zinc in it.  Especially galvanized material.  It gives off toxic fumes.
  • If you want to see the path the plasma cutter will take and check the positioning of your material without cutting it, leave the plasma cutter off.  Only turning on the computer and the controller will allow you to import your code and move the plasma cutter without it actually cutting the material.

REFERENCE

PROCEDURE

The general workflow for using the CNC plasma is as follows.

  1. CAD Design
  2. CAM toolpath creation
  3. Machine Setup and Control

There are many different software options that can be used to make it through this workflow. Langmuir provides extensive video tutorials that cover the full workflow using Fusion 360. This entire method can be followed on the Caroline computer, which has a Fusion 360 license. The most common workflow used at Vector Space is Inkscape -> SheetCAM -> Mach3.

1. CAD

There are a lot of options for creating 2D CAD drawings. Inkscape is the easiest, there's also FreeCAD and libreCAD.

2. CAM

The purpose of the CAM process is to provide the tool with instructions on how to create the CAD drawing. In the case of the plasma cutter, this typically means how to follow the lines, and at what speed. The three programs we've successfully used to do this are SheetCAM, FreeCAD, and pyCAM. Each is discussed below, but SheetCAM is recommended for beginners and can be found on the Caroline computer.

SheetCAM

The step-by-step instructions below assume that you have already created your object and are ready to improt it into SheetCAM to prepare the code for cutting with the plasma cutter.

Set post-processor to "Mach3  plasma"

  • Options -> Machine -> Post processor drop down to "Mach3 plasma"

Import your drawing

  • To begin a new project, Click the File menu – New Part.  If you want to import a previously designed object from another program (dxf, svg, etc.), in the pop-up menu that opens, choose Yes when it asks if you want to Import a drawing, and then select your file from the explorer menu.
  • Under the drawing options, pay special attention to Scaling and Position
    • Scaling: Default is set yo 0.5 which is roughly half the size of the imported drawing.  If you want it full size, change this to a “1”.
    • Position: Default is set to the bottom left corner.  This setting or any of the other corners would work best depending on if you have a blank piece of material.  If you set the position to center, the plasma cutter will always start from the bottom left corner of your material and move to the object.  If you are working around previous cuts, this makes the job much more difficult to position on the plasma cutter.
  • If you did not import a drawing file, you can create your object using the SheetCAM controls.

Creating and assigning layers

Once you have completed your design or finished adjusting settings for the imported object, you can create different layers for objects if you want them cut in a certain order.  For example, you may want the plasma cutter to cut the holes out first, then cut the rest of the design afterwards.  To do this the program has the ability to assign objects to different layers.

When choosing to create your layers, be sure to choose them in the order that you want them to be cut.  For example, choose the “Holes” layer first, and the rest of the design second.  Think about how each layer will affect the rest of the project.  Cutting the design first will probably drop it out of the material, so then it would be difficult to cut the holes after this happens.

  • The program will assign all objects to one layer initially.
  • To assign objects to a new layer, click the Mode menu and select Edit Contours.
  • Left click and hold, then drag the mouse over one or more objects and then release the button.  
  • Right click on any of the selected objects.  In the pop-up menu click Move to Layer, New layer (you will name it) or choose an existing layer to assign the object to a previously created layer.
  • To edit the options for each layer:
    • Click the Operation menu, Plasma Cut
    • Pay attention to the following options in the pop-up menu:
      • Contour method: Do you want the cutting to happen on the inside, outside, or middle of the path lines.  For example, you may want the holes to be cut on the inside, but the rest of the design on the outside.
      • Layer: Make sure you have selected the correct layer for the parameters you are setting.
      • Feed rate: The default for this is set to inches per minute (ipm), so if you wanted 20 mm/s, 40 ipm would be close to the same speed (47 ipm would be the exact same).
  • Click “OK”.  The path setting will now show up under “Operations” on the left sidebar off the program.  You can double click to edit them later if necessary.
  • When you have finished editing your object and adjusting settings for the layers, you can process the object to be run on the plasma cutter.

Processing your object

Once you have imported your object and adjusted the layers, it is time to process the image and create the code that will tell the plasma cutter how to cut the object.  The code you create here will be imported into the Mach3 program installed on the plasma cutter computer.

  • Click the File menu, choose Run post processor
  • Name your file and save as a G-code (XX.tap) file.  Note: Even if you try to add “.nc” to the end of this file type, it will still only be recognized as a “.tap” file.
  • You will now be able to inspect the G-code at the bottom of the program window.  If processed correctly, there should be X and Y coordinates in this code along with many G-code commands.  SheetCAM will add in the start and stop commands between objects automatically and display the cutting path with lines and arrows.
  • You will need to open the “.tap” file in notepad/mousepad and then click File, Save As and rename the ending of the file to “.nc” so that the Mach3 software on the plasma cutter computer will easily recognize the commands without issues.  If you load the “.tap” file you may experience issues where the cutter will stop due to some elements of the code.  Using and loading the “.nc” type file seems to eliminate any issues, even though the code is identical and unaltered.

FreeCAD

If the 2D CAD drawing is created in FreeCAD, the tool path generation can be created directly using the Path workbench. There are a number of good video tutorials available on using the path workbench; however, almost all of them assume that a 3D object is being created on something like a milling machine. The process for a 2D plasma cut is even simpler, and can in most cases be accomplished by creating a contour path of your sketch.

Import Existing 2D design

  1. Import dxf or svg into FreeCAD
  2. Select all shapes, draft workbench, convert bidirectionally between draft and sketch
  3. Select all sketches, Sketch workbench, merge sketches creates new sketch
  4. Delete all other shapes and sketches
  5. Path workbench

Create Original 2D design

  1. Use sketcher to create design
  2. Change to path workbench
  3. Set output file name and change processor to linuxcnc
  4. Edit default tool for 80 in/min horizontal, 20 in/min vertical, click OK
  5. Create profile based on edges. Add edges using Geometry tab.
  6. Preview toolpath using simulator button
  7. Export .nc file using the post-process button

PyCAM

PyCAM is an alternative option to using FreeCAD. It is a simpler tool, but far less versatile by comparison. To get started, you can either import an SVG from inkscape or import a DXF from FreeCAD.


3. Machine Setup and Control

The Langmuir tutorials explain how to setup the physical machine prior to cutting and how to execute the GCODE you created in the CAM process by using the Mach3 software. Always have a little extra material or get your material a little larger for testing before you start your final cuts.  Create a simple object such as a small circle to test cut on your material to see how it comes out.

  1. Set nozzle above workpiece with 1/8in shim
  2. Jog the cutter where you want it and set x and y zero in Mach3
  3. Load gcode
  4. Test the programming by clicking cycle start

Speed and Power

The following table has been developed in-house. Please add to it with any experience you have.

Material Thickness Speed (inch/min) Amperage (Amps)
Carbon Steel 1/8 in 75 45
  1/4 in 35 45
Aluminum 1/8 in 110 45
  1/4 in 60 45
  1/2 in    
Stainless Steel 1/4 in 30 45

TROUBLESHOOTING

  • Torch does not arc
    • Check that the ground cable is properly attached to the table or workpiece
  • Torch arcs but cuts out quickly
    • Check that the workpiece is level relative to the torch, meaning that the gap is consistent across the entire workpiece
    • Check and if necessary, replace the torch consumables
  • The back side of the cut is not clean
    • Adjust the power and speed

CROSSFIRE™ CNC PLASMA MACHINE TROUBLESHOOTING

PROBLEM POTENTIAL CAUSES SOLUTIONS
Plasma Cutter is not automatically firing or is mis-firing intermittently. Worn out electrode. Inspect electrode and replace as necessary.
Cut height is too high. If the pilot arc starts but does not transfer to the work piece, it is possible that the cut height is too high. Lower the cut height in 0.020" increments until continuity is achieved. Please consult your plasma cutter manufacturer for published cutting parameters for your specific model.
Ground clamp not making electrical continuity with workpiece. If the pilot arc starts but does not transfer to the work piece, it is possible that the ground clamp is not making continuity to the work piece. Inspect that the ground clamp is properly attached. Also inspect that the plate is not sufficiently rusted or has a coating that will prevent continuity.
Plasma cutter is damaged. Inspect that your plasma cutter is still working properly off of the machine. Remove the torch from the torch holder and perform a manual cut off of the machine. If the torch does not fire, it's possible that the plasma cutter or torch has malfunctioned and you will need to contact your plasma cutter manufacturer for resolution.
Torch wiring not hooked up correctly to Torch ON/OFF port on electronics enclosure Inspect that the two wires are plugged in correctly to the Torch ON/OFF output jack on the electronics enclosure and that full continuity is made.
Torch wiring not hooked up correctly to plasma cutter trigger or CNC port. Inspect that the wires going from the electronics enclosure at the Torch ON/OFF output jack are spliced in correctly to the plasma cutter torch trigger wires. You may need to use a multimeter to preform a continuity test by manually pulling the plasma torch trigger and testing for continuity between the two wires.
Electrical relay inside CrossFireTM electronics enclosure is malfunctioning. If all other solutions fail to produce proper automatic torch firing, it is possible that the electrical relay within the electronics enclosure is not working properly. Please contact Langmuir Systems and submit a support request.
Torch height offset is low in some areas of travel and high in others. Workpiece is warped. Most plate is not perfectly flat and it may be possible that your workpiece is warped. Use a straight edge to inspect the flatness of your plate. If your plate is slightly warped, we recommend using C-clamps to fasten your workpiece down to the slat bed or the machine frame when cutting.
Slag accumulation on slat bed. The table surface is established by the top surface of the slat bed which can become chewed up after repetitive cutting and slag accumulation. We recommend removing the slag accumulation from the slat bed to re-establish the original bed surface. If the slats are too worn, it may be necessary to purchase a new slat pack.
Gantry tube is not level to slat surface. If all other solutions fail, it is possible that the gantry tube is not level to the surface created by the slat bed. Please consult the Assembly Manual for the correct procedure for aligning the gantry tube.
Stepper motors are missing steps (stalling) during programmed motion. Debris on rail tube surfaces. Both rail tubes should be wiped down clean with a dry cloth before and after cutting to prevent the accumulation of dust and debris which can hinder motion.
Excessive friction between lead screws and lead nuts. Inspect the spring mechanism on both lead nuts to ensure that they are moving freely and are not bound up. Apply a light coat of oil or grease to the full length of both lead screws and jog the machine back and forth to evenly coat.
Damaged carriage roller bearings. Inspect the roller bearings on both carriages for obvious damage and replace as necessary.
Machine travel limit reached. When the machine travel limit is reached, it will cause the motors to stall. Please make sure that your program is not cutting outside the travel limits of the machine.
Torch carriage colliding with workpiece. Perform a dry run of your program to inspect a potential collision between your torch and the workpiece.
Loose stepper motor connection at electronics enclosure. Inspect the connection between the stepper motors and the electronics enclosure for a loose connection and fasten as necessary.
Damaged Stepper Motor or Motor Drivers. If all other solutions fail to fix this issue, please contact Langmuir Systems and submit a support request.
Excessive backlash (play) resulting in irregular cut geometry. Lead screw couplers are loose. Inspect that two couplers used on each end of the lead screw to ensure that a tight fit is achieved. Re-tighten as necessary.
Lead nut is worn or damaged. Inspect the lead nut to ensure that the threads are not damaged and that the spring tensioning mechanism is functioning properly. Replace lead nuts as necessary.
Loose fastener between the lead screw coupler and roller bearing. Inspect the fastener at the end of the lead screw coupler where it clamps to the bearing. Tighten as necessary.
Lead nut fasteners are loose. Inspect the fasteners that attach the lead nuts to the lead nut mounts. Tighten as necessary.
Communication lost between CrossFireTM machine and computer controller (Mach3). USB cable unplugged from electronics enclosure or computer. Inspect that the USB cable is properly connected to both the electronics control box and your computer.
Synchronization has timed out between USB breakout board and Mach3 Software. Sometimes the sync between the USB breakout board and Mach3 can be lost. This can be due to programs running in the background or if your computer goes to sleep while running. To fix this issue, restart Mach3 software to restore the sync.
Breakout board (BOB) is damaged. If all other solutions fail, it is possible that the USB breakout board is malfunctioning. Please contact Langmuir Systems and submit a support request.
CrossFireTM machine is not powering on. The machine is not receiving power. Inspect all power cords and the power inlet switch for connectivity.
The power inlet fuse is blown. Remove the fuse at the power inlet rocker switch and inspect for damage. Replace the fuse if damaged.
The electronics control box is malfunctioning. If all other solutions fail, it is possible that the electronics control box is malfunctioning. Please contact Langmuir Systems and submit a support request.

 

GENERAL PLASMA CUTTING TROUBLESHOOTING

PROBLEM POTENTIAL CAUSES SOLUTIONS
Excessive cut edge angularity (bevel). Plasma torch nozzle is worn. The most common cause for increased edge angularity is a worn nozzle. Remove your plasma torch from the torch mount and inspect the nozzle orifice for wear. Replace as necessary.
Moisture in the compressed supply air. Moisture in the supply air can result in decreased cut quality which can produce undesired edge bevel. Make sure that you have a water separator in line with your supply air going to the plasma cutter. Also ensure that this water separator is functioning properly and is not full.
Torch is not perpendicular to cut surface. Inspect that your torch is mounted properly in the torch mount and that the torch is aligned perpendicular to the workpiece surface. Re-align the torch carriage as necessary in accordance with the Assembly Manual provided.
Travel speed is too fast. An increased travel speed will not allow the plasma jet to cut fully down through the workpiece while moving. This causes the plasma column to lag behind while cutting which can produce excessive edge bevel. Slow your travel speed down in increments of 10IPM until the desired cut quality is achieved.
Plasma torch nozzle diameter is too large. Most plasma cutters have a range of nozzles that are rated for amperage. Typically the higher amperage nozzles will have a larger nozzle orifice diameter. This larger orifice can produce more edge angularity because the plasma jet is not as tightly focused when using a smaller nozzle size. We recommend lowering your amperage and selected a smaller fine cut nozzle if possible for your project to produce better edge angularity.
Incorrect cutting amperage. Incorrect cutting amperage can product either positive or negative edge bevel. Adjust your arc amperage in 3A increments until the desired cut quality is achieved.
Workpiece is warped. A warped workpiece can result in irregular cut angularity due to the fact that the torch is no longer perpendicular to the workpiece. Inspect your workpiece and clamp as necessary. If you are experiencing warpage while cutting on thinner material, we recommending cutting with a water table to eliminate this thermal distortion.
Improper cut height. Cut height can have an affect on edge angularity which can produce either a positive or negative edge bevel angle. Adjust the cut height either up or down in 0.030" to reduce edge angularity.
Excessive backside dross (slag). Slow travel speed. Backside dross can occur when cutting if the travel speed used is too slow. Try increasing your travel speed by 5 IPM increments until the amount of dross is reduced.
Cut height is too low. If the cut height is too low, this can cause more backside dross to form. Try increasing the cut height in 0.030” increments until the back side dross is reduced.
Cutting amperage is too high. If the cutting amperage is too high, this can cause an increase in the amount of backside dross. Try reducing the cutting amps in increments of 3A until the amount of dross is reduced.
Large nozzle orifice diameter. A larger nozzle orifice can result in an increased presence of backside dross. Consult your plasma cutter manufacturer for the availability of smaller nozzle sizes that are compatible with your cutting torch.
Excessive topside dross (spatter). Cut height is too high. Top spatter or top dross can occur when the plasma stream first pierces the work piece and the molten metal adheres to the top surface of the material. It is typically much less common than back side dross and it can be easily removed by chipping away from the work piece. If you are experiencing a high incidence of top dross, it is possible that your chosen cut height is too high and should be reduced.
Pierce delay is too short. If the pierce delay is too short, it does not allow the plasma arc enough time to correctly pierce the material completely before motion begins. Try increase the pierce delay in 0.1 second intervals until top dross is eliminated.
Amperage is too low. If the amperage is too low, the plasma cutter does not have enough power to quickly pierce the material. Try increasing the cutting amperage in intervals of 3A.
Cut holes are excessively tapered. Travel speed is too fast. When cutting holes, the plasma cutter is constantly changing direction which can make it difficult to achieve a full speed cut in smaller holes. If you are experiencing holes that measure larger on the top surface than the bottom, it may be necessary to cut these holes out at a slower travel speed. We recommend programming a second layer in SheetCAM for your part and putting holes in the second layer at half of the desired travel speed.
Excessive edge angularity on part. Holes typically have higher edge angularity than straight edges. If you are already experiencing high edge angularity on the rest of your part, this will make holes even worse. Please refer to the above section on edge angularity for more troubleshooting tips.
Workpiece experiences a large amount of distortion when cutting. Thermal gradients established in workpiece during cutting. The plasma cutting processes uses a high temperature plasma arc to melt and cut through the workpiece. As a result, the workpiece will heat up locally which can establish a thermal gradient in the part. This gradient can lead to distortion which will effectively warp you workpiece. Typically with material that is 3/16" and thicker, distortion is not as much of an issue because the plate is strong enough to resist this warping. On thinner plate and sheet metal, distortion can be an issue which can make detailed cutting impossible without distorting the workpiece.


Fortunately, some cooling methods can be used that completely eliminates this distortion when cutting. A water table is simply a tray filled with water that surrounds the slat bed of a gantry-style CNC plasma machine. The tray is filled with water to below the top surface of the slat bed so that the action of plasma cutting causes water in the tray to splash back up onto the backside of the part being cut. This allows for part cooling, reduces cutting noise, decreases part warpage, reduces arc flash, and reduces smoke and cutting dust. A water table can be purchased for the CrossFireTM machine from Langmuir Systems or it can be made by following our guide in the Projects page. If you are not able to purchase a water table, we have had an equal amount of success by using a standard spray water bottle and continuously spraying the plasma arc with the water bottle during cutting to cool the part.

Cut does not penetrate completely through workpiece. Amperage is too low. If the plasma cutter amperage is too low, it will not have enough power to completely penetrate the material. Try increasing the amperage in 3A intervals until a clean and complete cut edge is achieved. Consult your plasma cutter manufacturer for proper amperage settings for your machine.
Travel speed is too fast. If the travel speed is too fast, the plasma arc will lag behind and will not be able to complete several the material. We recommend slowing down the travel speed in 10 IPM increments until a satisfactory cut edge is achieved.
Supply air pressure too low. If the supply air is too low, it will not have enough power to completely sever the material and will result in a poor cut edge. Consult your manufacture for the correct supply air pressure settings and make sure that your air compressor has enough capacity to keep up when cutting.
Cut height is too high. If the cut height is too high, the plasma arc may not penetrate completely through the material. Try lowering the cut high in 0.030" increments until a complete severance cut is achieved.
Consumables are wearing out more quickly than expected. Nozzle orifice is clogged or dirty. The daily buildup of dirt and grime on the nozzle can clog the orifice which greatly affects the swirling of the plasma arc. This can lead to decreased lifetime for both the nozzle and electrode. Make sure that the plasma nozzle remains clean before each use.
Supply air pressure is incorrect. If air pressure is too high, this can greatly reduce the lifetime of the electrode. Conversely, if air pressure is too low the nozzle orifice will wear which can affect cut quality. Consult your plasma cutter manufacturer for ideal air pressure settings for your specific plasma cutter model.
Cut height is not set correctly. When the plasma cutter initiates the arc, it can take several moments to completely pierce the material depending on the thickness of the material. During this pierce, molten metal is ejected from the topside of the material which can be blown back onto the nozzle orifice. As a result, it is important to use a cut height that is not too low to avoid this blow back of material which can damage the nozzle orifice over time. Conversely, if the cut height is too high the arc will not transfer which will degrade the lifetime of the electrode. Consult your plasma cutter manufacturer for the correct cutting height parameters for your given project.
Supply air is not dry. The plasma cutting arc is especially sensitive to moisture. Air compressors take humidified air from the atmosphere which always contains some amount of water. Make sure that you either have a water separator on your plasma cutter or that you have a water separator in line with your air compressor before the air is delivered to your plasma cutter. Moisturized air can greatly decrease the lifetime of your consumables and can negatively affect cut quality.
Incorrect cutting parameters. Every plasma cutter is different. We encourage you to contact your plasma cutter manufacturer to get a complete list of proper cutting parameters to use with your machine to optimize the lifetime of your consumables.
Unequal (uni-directional) edge angularity. The workpiece is warped. If a workpiece is warped, it can cause a unidirectional edge bevel because the plasma arc is not perpendicular to the material surface. Inspect the material for flatness and use clamping as necessary.
The torch is not mounted perpendicular to the slat bed surface. Inspect that your torch is mounted properly in the torch mount and that the torch is aligned perpendicular to the workpiece surface. Re-align the torch carriage as necessary in accordance with the Assembly Manual provided.
Slag accumulation on slat bed creating an unequal cut surface. The table surface is established by the top surface of the slat bed which can become chewed up after repetitive cutting and slag accumulation. We recommend removing the slag accumulation from the slat bed to re-establish the original bed surface. If the slats are too worn, it may be necessary to purchase a new slat pack.
The gantry tube is misaligned. If all other solutions fail, it is possible that the gantry tube is not level to the surface created by the slat bed. Please consult the Assembly Manual for the correct procedure for aligning the gantry tube.
Irregular cut geometry along one axis. Incorrect stepper motor settings in Mach3. If the motor tuning settings are changed accidently in Mach3, it can affect the 'gear ratio' for a given axis. If this happens, you will need to re-load the specific Mach3 configuration file for the CrossFireTM machine. Please consult the Assembly Manual for instructions on how to configure Mach 3 for your machine.
One lead screw coupler is loose. Inspect that two couplers used on each end of the lead screw to ensure that a tight fit is achieved. Re-tighten as necessary.
Lead nut is worn or damaged. Inspect the lead nut to ensure that the threads are not damaged and that the spring tensioning mechanism is functioning properly. Replace lead nuts as necessary.
Loose fastener between the lead screw coupler and roller bearing. Inspect the fastener at the end of the lead screw coupler where it clamps to the bearing. Tighten as necessary.
Lead nut fasteners are loose. Inspect the fasteners that attach the lead nuts to the lead nut mounts. Tighten as necessary.
Part dimensions are oversized/undersized compared to design. Kerf width setting is too large. If the kerf width setting for your programmed tool in SheetCAM is too large, the dimensions of all outside offset part geometry will be undersized (all inside offset geometry will be oversized). We recommend making a test cut at the known parameters in a straight line and using a tape measure or caliper to measure the actual kerf width.
Kerf width setting is too small. If the kerf width setting for your programmed tool in SheetCAM is too small, the dimensions of all outside offset part geometry will be oversized (all inside offset geometry will be undersized). We recommend making a test cut at the known parameters in a straight line and using a tape measure or caliper to measure the actual kerf width.
Divots' created in cut edge at starts/stops. Missing or under-sized cut lead-in. Lead-ins are used when CNC plasma cutting in order to make smooth cuts when piercing a material. A lead-in is used at the start of a cut so that the plasma arc can be pierced in an area of the part that is slightly away from the actual geometry of the part. After making the pierce, the plasma torch moves along the lead-in path (usual an arc) and makes a smooth cut around the part geometry. Without a lead-in, a rough cut or 'divot' will result where the plasma torch first made the initial pierce since it pauses here for a given amount of time when piercing.
Excessive gap between part and slat surface. Sometime 'divots' in the cut edge can result when a cut is finished and the part starts to drop out before the cut is completely finished. This usually happens when the drop is small enough so that it is unsupported by the slat bed when the cut is complete. To avoid this, make sure that the drop is supported when the cut is complete.


                                 END OF THE PROCEDURE