Waterjet Class
Enroll
Lesson 2: Software for the Waterjet
Ask a Question Download

Introduction: Software for the Waterjet

You will need two pieces of software to use the waterjet. One will prepare the file for cutting, and the other will control the machine.

To prepare the file, you can use the 2D Pathing Tool in Fusion 360 or Omax Layout to prepare a DXF or Illustrator file.

Omax Make is always used to operate the machine.

CAM Mode in Fusion 360

Fusion 360 can create Omax-ready files natively.

For using Omax Layout, skip to the bottom of this lesson or page 12 in downloadable .pdf from this lesson

Get ready

1. Go into CAM mode.

2. Check your units in the tree.

  • Make sure you are working in the correct units.

Create a New Setup in Fusion 360

  1. Click the New Setup button.
  2. Select Cutting from the Operations Type menu in the Setup tab.
  3. Select Select Z axis/plane & X axis from the Orientation menu.
  4. You need to select the Z Axis.
    • Click on the top plane of your part and ensure that the blue Z arrow is pointed up.
  5. The X axis arrow should be pointing to the right.
    • Click the red x to flip the X axis if needed.
    • Or you can select the Flip X Axis checkbox.
  6. Select Selected Point from the Origin menu.
  7. Click on the lower left point of your model.
    • Double check that the Z arrow is up.
    • The X arrow should be to the right.
  8. Click the top plane of the model.
    • The Model menu should change to Body and the top of the model should be blue to show that it has been selected.
    • Double check that the model looks like it will cut correctly.

Define the Stock in Fusion 360

Input the stock size

1. Click the Stock tab.

2. In the Mode menu, select Fixed size box.

In the next steps, you'll enter the size of the stock, and how far from the edge your part is. Be sure to set Z (material thickness).

3. Set the stock dimensions and the position.

  • In this example, the stock is 5" wide and the part starts .25" from the left edge.
  • The stock is 5" high and the part is offset .25" from the bottom.
  • The stock thickness is .25" and there is no offset; the part completely fills the height of the stock.

4. Check that the stock thickness is correctly displayed at the bottom of the dialog box and click OK.

Tool Libraries in Fusion 360

ADD THE WATERJET TO THE TOOL LIBRARY

In order to select the waterjet as a cutting tool, you'll need to add it to your tool library in Fusion 360.

  1. Click the Manage Tool Library button.
  2. Click the Waterjet/Laser cutter icon in the upper right.
  3. Click the Cutter tab.
  4. Select Waterjet in the Type field on the left.
  5. Enter the Kerf Width on the right.
    • The Kerf Width is equal to the diameter of the nozzle.
    • It is noted on a sticker on the control computer.
  6. Click the Feed & Speed tab
  7. Select Machine uses quality in the Feedrates menu.
  8. Click OK.
  9. Close the Tool Library window

Creating Toolpaths in Fusion 360

The next step is to tell the waterjet where to cut.

Click the CUTTING button

Select the tool

  1. Click the Tool tab.
  2. Click the Tool button to select a tool.
  3. Select Waterjet In the dialog that opens and click OK.
  4. Select the desired quality in the Cutting Mode box.

Select the features to cut

  1. Click the Geometry tab.
  2. Click each feature you want to cut.
    • Another option is to click Select same plane faces and click the face of the part.
    • This will select all the features on that plane.

Tabs

Tabs are short gaps that don’t get cut, in order to keep small parts attached to the workpiece. The tabs prevent the piece from moving during the cut or falling into the tank.

  1. Click the Tabs checkbox.
  2. Select At points in the Tab Positioning box.
  3. Click to place tabs.
    • Usually two or three tabs will keep a piece from moving.
    • Place the tab in an area that will make it easy to remove, such as on a straight section. A tab in a tight corner may be difficult to remove.
    • Be sure to place the tab on the waste side of the part.

Heights

USE SAFE HEIGHTS TO AVOID BREAKING THE NOZZLE.

Setting the height of the nozzle helps to keep from breaking it on clamps and other objects. Make sure you set the nozzle high enough to protect it.

You will need to set the height for two different things

  • Clearance Height
    • The distance above the workpiece at the start of a new toolpath.
    • Make sure this is high enough to avoid clamps.
  • Retract Height
    • The distance above the workpiece when the nozzle is moving between cuts (also known as a traverse).
    • Make sure this is high enough to avoid clamps.

  1. Click the Heights tab.
  2. Set the Clearance Height.
    • By default, this is added to the Retract Height.
    • For example, if your Retract Height is 0.5" a 1" Clearance Height will give 1.5" of clearance.
  3. Set the Retract Height.
    • By default, this will be measured from the top of the workpiece.

Simulation and Post in Fusion 360

SIMULATE THE CUT

Simulating the toolpath will allow you to check for errors and collisions.

  1. Select the part by clicking the 2D Profile in the tree.
  2. Click the Simulate button.
  3. Use the controls at the bottom to run the simulation.

POST PROCESS

The post-processor will write the machine instructions for the Omax, and save the le.

  1. Click the Post Process button.
  2. Select Omax from the Post Configuration menu.
  3. Click Post.
  4. Name and save the le to a thumb drive.

NEXT STEPS

Take your thumb drive to the waterjet, and skip ahead to Using Omax Make further down in this lesson, or page 17 in the printout (available in the last lesson) .

Creating Toolpaths in OMAX Layout

USING OMAX LAYOUT WITH DXF AND ILLUSTRATOR FILES.

For instructions on using Fusion 360 CAM for the Omax see the beginning of this lesson, or page 6 in the printout (available in the last lesson).

OMAX SOFTWARE TIPS - RIGHT CLICKING

Any icon that has a small red triangle in the upper right will allow you to right-click to choose an optional command.

  • For example, the Select button will default to Cursor when clicked. When right-clicked, it will show you a menu of selection options.
  • One of the menu commands will be Help, which opens a detailed help screen for that command.

MENUS

There are menus at the left, right and bottom of the screen, in addition to the standard menus at the top.

  • Edit
    • The Edit menu is on the left side of the screen, and has options for selecting, moving, copying, etc.
  • Draw
    • The Draw menu is directly below the Edit menu. It can be used to draw primitive shapes. However, it's much more simple to draw in CAD, Illustrator or other vector software.
  • Special
    • The Special menu is on the right side of the screen, and is used for toolpaths and cleaning the vector file.
  • View
    • The view menu is at the bottom of the screen, and has options for cut quality, undo and measuring.

Preparing Your File in OMAX Layout

IMPORTING A DXF FILE IS USUALLY THE BEST OPTION

Open the file

  1. Open your file with Import from other CAD... from the File menu.
  2. Leave the default boxes checked.
  3. Click OK.

Clean the geometry

Some vector files are imported with errors, such as gaps or duplicates. This step will solve most of the problems.

  1. Click the Clean button in the Special menu on the right side.
  2. Select all the boxes in the dialog box.
    • The Remove unclosed paths checkbox can be left unchecked if you have geometry with open ends (a line instead of a loop).
  3. Click Start.

Check the size

Sometimes drawings are imported with incorrect units. Since each square in the grid represents an inch, it's simple to check if your vector file was imported with the correct units.

Change the size if needed

  • Right-click the Select button, and choose All.
  • Right-click the Size button for sizing options.

Move the geometry

You may need to move your geometry onto the grid.

  1. Click the Move button in the Edit menu.
  2. Click the geometry to select a start point.
  3. Move the geometry until it is inside the grid, and close to the lower left corner (home).
  4. Right-click Deselect in the Edit menu, and select All.
    • If the geometry is yellow, it is still selected.

Line Types and Quality in OMAX Layout

EACH LINE IN THE DRAWING NEEDS TO BE ASSIGNED A VALUE.

Quality & line types

You will need to assign a type or value to every line in your geometry. The quality of the cut can be assigned a value from 1 (lowest quality) to 5 (highest quality). Lower quality cuts will take less time and use less garnet, but produce a rougher cut. Each quality is represented by a different color on-screen. Other colors represent different types of lines.

Each line in your drawing will need to be assigned one of the values from below.

  • Quality (1-5)
    • Quality 3 is a good compromise of speed vs. quality for most cuts.
    • Thicker material shows the effects of a low-quality cut more than thin material.
  • Traverse - Do not use
    • The head will move from the end of one cut to the next.
  • Heads Up Traverse - Use this move
    • This is like a regular traverse move, but the head will raise up several inches.
  • Etch
    • This is a mix of water and garnet that will etch the surface, but not cut.
  • Scribe
    • Scribing is like etching, but without using garnet.
  • Water Only
    • This is a cut, but without the garnet.
  • Lead In/Out
    • These are short lines that start (and stop) the cut away from the cut line.
    • The initial pierce of the jet can distort the material; starting and stopping the cut in a waste area hides the damage.

Set line quality

The menu on the bottom of the screen allows you to assign a quality to each line.

  1. Right-click Quality to bring up the submenu.
  2. Choose your selection method.
    • This works like the Select button.
  3. Choose the quality level for the selected lines.
    • For the 5 levels of cutting, you can right-click and select slit, which is a cut directly on the line, rather than offset to one side.
  4. Right-click Deselect in the Edit menu, and select All.
    • This will show the line quality color.

Lead In/Out and Tabs With OMAX Layout

USE TABS TO KEEP SMALL PARTS ATTACHED TO THE WORKPIECE.

Check your work

After assigning line quality, deselect all. Each line will be assigned a color that represents a type of cut or traverse.

Note: Use Heads Up Traverse (dashed green lines).

Make the Lead In/Lead Out lines

  1. Right-click Lead i/o from the Draw menu.
  2. Select AutoPath (Advanced & Configure)... from the sub-menu.
  3. The left side of the window allows you to select tool path options.
  4. The right side displays your file and toolpath.

On occasion, a small cutoff piece can flip up and come in contact with the head. Choosing a toolpath that has fewer possible collisions is best practice. In some cases, it may be required to create custom Lead i/o lines. See Shop Staff.

The start and end of the toolpath can be changed by selecting any of the 9 green (start) or red (stop) buttons.

  • It is common to start the toolpath in the lower left corner.

Click Go! to save your settings.

Tabs

Tabs are short gaps that don’t get cut, in order to keep small parts attached to the workpiece. The tabs prevent the piece from moving during the cut or falling into the tank.

  1. Right-click Lead i/o from the Draw menu.
  2. Select Create Tab from the submenu.
  3. As your mouse approaches a cut line, the tab will jump to the line.
  4. Click to place the tab.
    • Usually, two or three tabs will keep a piece from moving.
    • Place the tab in an area that will make it easy to remove, such as on a straight section. A tab in a tight corner may be difficult to remove.
    • Be sure to place the tab on the waste side of the part.

Toolpath and Inspection in OMAX Layout

Create the toolpath

  1. Click the Path icon in the Special menu.
  2. Your cursor will change to a + and the words “PICK START”.
  3. Click the beginning of the lead in line that you created earlier.
    • This should be lower left, outside of your cutting area.

Inspect the toolpath

Inspect the toolpath to ensure that you’ll be cutting on the correct side of the line.

Your cut line will be displayed in the color that corresponds to the quality, and traverse lines will be green.

The thick red line with a dotted center displays two things:

  • Dotted center
    • Displays the actual path of the jet.
  • Thick red line
    • Displays the kerf (the material removed by the jet).

If the toolpath is cutting on the wrong side of the line, there are two common possibilities:

  • There’s a gap in the geometry.
    • Follow the toolpath by eye and look for a gap where the toolpath doubles back on itself.
    • Fix the gap with the provided tools and re-create the toolpath.
  • The software chose the incorrect side to cut on.
    • Right-click the Lead i/o button and select Swap Lead Direction.
    • Click to select the lead in line to be swapped.
    • Recreate the toolpath.

Save the file

When you are happy with the results, click the save button.

The file should be saved as an ORD (Omax Routed Data) file, which can be opened in Omax Make.

Using OMAX Make

  • Open Omax Make from the desktop.
  • Select File > Open (Change Path Setup)...

Opening a part with Omax Make

The Open File dialog box has three panels you should pay close attention to.

  1. File Navigation
  2. File Preview
  3. Material Settings


Open the part

  • Use the File Navigation Panel to open your ORD file.
    • Confirm you have selected the correct file with the preview.

Select your material

  1. Select your material from the list.
    • Materials are listed by category (metals, woods, plastics...).
    • If your exact material is not on the list, see Shop Staff.


Set the material thickness

  1. Use a digital caliper to measure the thickness of the material.
  2. Enter the value in decimal inches.
  3. Click OK.

The software is now ready to control the waterjet and cut your parts.

Notes on increasing the accuracy of the cut:

As the mixing tube wears, the kerf will grow larger. If your parts need to be held to a tight tolerance, you may need to adjust the Tool Offset.

Cut a 1" square from your material and measure it with calipers or a micrometer. If it is undersized, increase the value in the Tool Offset eld by 1/2 the error.

For example, if your 1.000" circle measures 0.998", increase the tool offset by 0.001".