Plasma First Cuts: Programming Toolpaths¶

Software Note

Before starting these next steps, make sure that you have already downloaded and configured SheetCam on your computer. For further details on the install process, please refer to these instructions.

The steps included below will walk you through how to transform your vector file into a machine-readable code. Unlike the workflow for our CNC routers, our Plasma CNCs require that you import your design files to SheetCam, a powerful plasma CAM package.

The G-code file you will create using this program will include all the motion information that the machine needs to cut your design successfully. The G-code header will also include the information for your programmed material type, material thickness, torch type, and amperage.

Use the checklist below to monitor your progress while working in the SheetCam:

Step 1: Define Machine Dimensions
Step 2: Define Material Dimensions
Step 3: Import and Place Vector Drawing
Step 4: Create a New Jet Cutting Operation
Step 5: Select Lead Ins and Lead Outs
Step 6: Enable THC Code
Step 7: Edit Lead Locations
Step 8: Configure Cutting Operations for Additional Layers
Step 9: Save Your File

Step 1: Define Machine Dimensions¶

The light gray rectangle in your SheetCam window represents the size of your machine bed. Utilize the steps below to update its dimensions.

Navigate to "Options > Machine."

Select the Working Envelope tab in the window.
Edit the values listed in the X and Y text boxes so that they align with the length and width of your machine.
Save by clicking "OK".
The light gray box will then resize to the new inputted dimensions.
After you complete this step for the first time, your inputted dimensions will remain static unless you manually update them again.

Step 2: Define Material Dimensions¶

The red box in the SheetCam workspace represents the size of your cut material. Before uploading your design, these dimensions will also need to be updated.

First, navigate to "Options > Job Options"

In the Material tab, edit the X and Y values so that they accurately reflect the dimensions of your cut material.
Note: Changing the material thickness in this window does not impact your cutting operation. You will set the material thickness later while configuring your toolpaths.
After clicking "OK" the red box in the workspace will resize to the new inputted dimensions.

Step 3: Import and Place Vector Drawing¶

Now that the machine bed and material dimensions are updated, you are ready to import your design.

Navigate to File > Import Drawing

Select the DXF file you wish to use and click "Open".

After clicking "Open" the Drawing Option window will be displayed. Confirm that the units selected are the same ones you used in your design file.
In the same window, use the Drawing Position diagram to select where you would like your design to be placed.

After hitting "OK" the design will appear in the red material profile box, snapped to the origin point selected in the previous window.

You can then reposition your drawing by selecting the Nesting Tool in the toolbar.
We highly suggest offsetting your design from the material edge. Programming the cut beyond the material can lead to incomplete parts and loss of arc.

The layers you created in your vector software will also be imported and listed in the Layers menu.

Step 4: Create a New Jet Cutting Operation¶

Once your drawing is imported and positioned where you want it, you can move on to setting up your tool paths.

IMPORTANT NOTE

Before you start this next step, spend some time considering the order that your design elements should be cut out.

If your design has any details nested within a larger profile, you will want to ensure that the details are cut out FIRST.

If the profile is cut first instead, there is a possibility that the part will fall into the water table before the details are cut.

SheetCAM typically does well differentiating internal/external features - cutting internal features first, followed by external features. If control by layer is desired, the easiest way to set up layers is in your vector software of choice.

Please review the Design Instructions to learn more about setting up layers in VCarve, Adobe Illustrator, and Inkscape.

Navigate to the Create A New Jet Cutting Operation icon in your Operations window.

After selecting the icon, the Jet Cutting window will be displayed.

Utilize the Contour Method drop-down to select your tool path offset.
This function allows you to specify if you would like the torch to cut on the inside, outside or on the line of your vector drawing.

Sheetcam_Tool_Settings_Contour_Illustration

For details nested within other profiles, inside offsets are generally recommended. For profile cuts, outside offsets are recommended (see illustration above).
In our example drawing, the Details layer (the one that contains the A, V, I, D and small circles) should be set to Inside Offset.
The Profile layer (the one that contains C, N, C and the rectangle) should be set to Outside Offset.

Next, use the Layers drop-down to select the layer you would like to cut first. If you only have one layer, still confirm that it is selected in this drop-down.

Select your material type, thickness, torch type and consumable type by utilizing the Tool drop-down.
Your selection in the Tool drop-down will automatically update your tool settings based on the ones pre-programmed in your Tool Library.

Software Note

If you do not see your Tool Library in this drop down, refer to these instructions).

If you would like visibility into the tool settings, click the ellipsis ... button to the right of the drop-down.
You can then use the resulting Jet Tool window to confirm or change the auto-populated settings.
Refer to the cutting charts in your Hypertherm Owner's Manual for more details on how to modify these settings for a given job.

Use the Path Rules drop-down to select "Default."
For further visibility into the Path Rules settings, click the ellipsis ... button to the right of the drop-down.
For further details on path rules, please refer to these instructions).

Step 5: Select Lead Ins and Lead Outs¶

An additional setting to consider in the Jet Cutting window is your Lead In and Lead Out controls. When a torch starts a new cut, it dwells at the start location in order to pierce fully through the material. This causes a small round mark or "scar" at the initial pierce location (see photo below for an example).

Lead ins and lead outs help mitigate the impact of scarring by starting the initial pierce away from your cut line. They also ensure that your part is fully cut out.

In the Lead Ins and Lead Outs section, select the Arc option for both.
Depending on the size of your cuts, you may want to adjust the length of your leads in order to fit them within the profiles. Do not go smaller than the thickness of the material.

Programming Note

Leadouts on internal features (holes, cutouts, etc.) can cause torch height control issues. Once the cut passes the start point, the material may fall and the leadout will have nothing to cut. This depends largely on the feedrate (thickness).

Thin materials require faster feedrates which may cut some material before it falls through. Thick materials with slow feeds have a greater chance of the "hole" falling in before the leadout actually cuts.

If this is not accounted for with path rules, the torch may dive.

In some cases, a small amount of overcut (~0.050") may be a better programming stategy for internal features.

Step 6: Enable THC Code¶

The last setting in the Jet Cutting window is the Use Code Snippet drop-down. This option will ensure that lines of code needed to operate Torch Height Control (THC) are included in your exported file.

THC is a powerful tool that helps modulate the height of your torch during a cutting operation. While you will be able to refine THC settings further in Mach4, make sure to enable it during this step.

Utilize the Use Code Snippet drop-down to select "Code: Code, M62P4 (+++THC Allowed, AD2 +++)".

After clicking "OK" in the Jet Cutting window, the new tool path will be overlaid on top of your vector drawing.
The tool path will also now be listed in the Operations Menu in the lower left corner.

Step 7: Edit Lead Locations¶

Occasionally, SheetCam will automatically assign leads in tight corners and small curves. These placements have the potential to negatively impact the quality of your cut.

For that reason, make sure to review your lead placements carefully and move them if necessary.

Select the Edit Start Points in your toolbar.
Click on a lead, and then click on the location you would like it to be moved.
For best performance, note the direction of the cut arrows and then place the lead at the start of a long, straight segment.

Step 8: Configure Cutting Operations for Additional Layers¶

If necessary, repeat the Create A New Jet Cutting Operation process for the other layers in your design.

Any new operations will also be saved in the Operations menu.
You can always rearrange their order by clicking and dragging the operation you would like to move to a new position.

Step 9: Save Your File¶

Once cutting operations have been configured for all layers, refer back to your checklist. Before saving your file, confirm that the following steps are complete:

Step 1: Define Machine Dimensions
Step 2: Define Material Dimensions
Step 3: Import and Place Vector Drawing
Step 4: Create a New Jet Cutting Operation
Step 5: Select Lead Ins and Lead Outs
Step 6: Enable THC Code
Step 7: Edit Lead Locations
Step 8: Configure Cutting Operations for Additional Layers

If you are able to check off Steps 1-8, move on to the next step.

Navigate to "File > Run Post Processor."

Name your project, confirm that the file will be saved as a .tap file, and click Save.

Next Steps

After saving your program, continue to Step 3: Machine Startup