Programming a part from a DXF (OMAX Maxiem 1515)

To cut a file on the waterjet you must first run it through OMAX Layout and tell it where you wish to cut. It's relatively straightforward but the software can look complicated if you haven't used it before.

Start with a DXF file

Most of the time you will need a flat, 2D file to use with the waterjet cutter. You can either draw this directly in Adobe Illustrator, or you can export it from software such as Fusion 360 or Solidworks.

• Exporting drawings as DXF files from Solidworks
• Exporting faces as DXF files from Solidworks
• Exporting sketches as a DXF file from Autodesk Fusion 360
• Exporting DXF files from Adobe Illustrator

Opening the file in OMAX Make

	Select File > Import from other CAD Don't choose File > Open, this is for opening files that you have previously created with OMAX Layout.
	A window pops up showing a preview of the file you are importing. The defaults on this page are typically fine, but if you run into problems further down the line with missing geometry take a look at the filter options here.
	A window will pop up asking if you wish to import the file as metric (millimeters) or imperial (inches). Look at the dimensions this window is offering you - if you have a part which is dramatically oversized, such as 30 inches wide when you are expecting something 30 mm wide, then you should scale down to metric. If your file has been drawn in millimeters you should click Yes.
	Use the Measure or Inquire tools in the toolbox at the bottom of the screen to check a known dimension on your part. With the Inquire tool you can click on a line and it will tell you the length, with the Measure tool it will tell you the distance between two points you click on.
	Select Clean from the right hand toolbox. It's important to clean your drawings before starting work on them - this will clean up any gaps or overlapping geometry, and convert segmented curves into continuous smooth arcs.
	The defaults are typically OK, so you can click Start. Check the state of any holes and curves after running the cleanup operation - you may find they have distorted. In which case, either adjust the position of the circles slider at the bottom or uncheck the box. If you find you're having problems when trying to post process your file it's probably because you forgot to clean your drawing at the beginning.

Setting up the toolpaths

	Automatically creating the toolpath with Autopath will work for 99 out of 100 jobs, but you do need to tell the software where you want to start and finish your job. Right click on Autopath in the left hand toolbox and select Autopath (Advanced & Configure).
	Select the start point and end point using the buttons on the left hand side of the Autopath window that appears. The green diamond is the start point. The red circle with a black triangle inside is the end point. Use the start point strategically to get the most out of your material. Click Go! to automatically create the toolpath for your part.
	If you part is small (typically under 100mm in the X axis) you should strongly consider using tabs to keep your part attached. A tab is a small section of the perimeter that will not be cut, keeping the part attached to the parent stock until you remove it. Right click on the Lead i/o button on the left hand toolbox and select Create Tab from the menu that appears.
	Hover over the purple cutting path you want to create a tab on. A tab will appear, and you can reposition it by moving the mouse along the path. If you wish to modify the size of the tab click the Options button that has appeared in the bottom left of the window. Click the line to create the tab. Don't add too many tabs, or you may find it is difficult to remove your part.

Post-processing ready for OMAX Make

	When your design is ready, left click on the Post button in the right hand toolbox. The cursor will change and ask you to Pick Start. Click on the end of the green line in the start position you chose earlier. In this case the start point was set to be the bottom left of the drawing, so I will click the end of the green line in the bottom left.
	In the new window that appears check that the dashed pink line is on the correct side of the line - this indicates the kerf of the waterjet and should be on the inside of holes and outside the perimeter of your part. Click Check for problems. Ideally your program will have zero issues, as indicated by the report in the top left of the window. If there are a lot of errors, especially offsets set to the wrong side, check that you selected the correct start point when prompted earlier. If there are potential collisions, right click on Check for problems and select Convert collisions to heads-up. This will raise the head up automatically when traversing over areas that have already been cut to avoid potentially tipped-up parts. If everything is fine, click Save. If there are issues, click Reject and try again after making corrections.
	Once you have saved your post-processed file you can open it in OMAX Make. Right click on Post Process in the right hand toolbox, and select Open ORD Path in MAKE... Select Retry in the message box that appears. OMAX Make will now open and you can set the material settings for your cut.