________________________________________
Creates the tool path (OMX file) needed to make a part
The Generate Tool Path command creates the tool path as an OMX file used by GlobalMAX to machine a part. The tool path must be one continuous path, although the abrasive jet can be turned off for parts of the path (using the traverse Quality).
After the tool path is generated, a preview of the tool path will appear. Examine the path, zooming in to ensure that the results are satisfactory. The preview can also display the kerf for the part. The tool path is not saved until you click on the Save button.
Only order each part once. If a change is made to the part, however, order the part again, or the new changes will not be incorporated when the piece is made.
Before you generate the tool path, you can use the Clean command to "clean-up" the drawing. This process will detect common drawing mistakes (such as lines that are on top of each other) and correct them.
By choosing Automatically Generate, either by selecting it from the right-click menu, or by left-clicking on the Path button, the tool path will be generated with the last set of options used in Custom tool paths. Changes to the Custom tool path options are stored and used for automatic generation.
If the custom tool path options have never been changed, the following options are used:
- The tool path is always offset to the left by the kerf amount.
- Entities with endpoints less than 1/1000th of an inch are considered connected.
- The tool path file has the same name as the part file, but with the extension (the part of the file name following the period) OMX.
- The computer will make all decisions about which direction to go when entities intersect.
If these are not the options desired for making a part, use Custom tool path options to create the tool path.
If these options are acceptable, however, quickly and easily generate the tool path simply by indicating the beginning of the path. LAYOUT will take care of the rest.
1. Click the Path button.
The screen changes to display the drawing full screen. A Zoom toolbar also appears.
The cursor changes to remind you to click on the start of the tool path.
The Zoom toolbar
Click on the start of the tool path
2. Click (or near) the start of the tool path. LAYOUT begins creating the tool path.
Use the Zoom toolbar to zoom in for a closer look at the point you want to use. If the part is complicated and you want to stop generating the tool path, click on the Cancel button. (With smaller tool paths, LAYOUT is usually done before you can cancel the operation.)
3. A dialog appears with the preview of the tool path.
A preview of the tool path
Path Preview
This main window shows what the tool path will look like.
Tool Offset to show
The size of the offset. Change this to match the offset of your machine, giving an accurate view what the finished part will look like. If there are inside curves that are smaller than the tool offset, an error message appears in the upper left corner of the preview dialog. The locations where problems are encountered are highlighted in yellow, to help you locate them.
The yellow highlights curves that are too small for the current tool offset
Offset Leads
When this is checked, lead-ins and lead-outs on the part will also be offset. Usually, this is the correct setting. In some situations, where precise control over the location of the leads is required, offsetting them might not be desirable.
Save Path
Save the tool path with the same name as the drawing file, assigning it an extension of OMX.
Right-click on the Save button, and you can use a different name for the tool path. You can also save the offset tool path as a DXF file, which you can then load into LAYOUT and modify--giving you unlimited control over the path.
After saving the file, you are returned to the main LAYOUT screen.
Reject Path
Click on the Reject button, and the tool path is not saved. You return to the main LAYOUT screen.
Right-clicking on the Reject button brings up a menu with additional choices. You can choose to reject the tool path, but select those elements that made it into the path. This is useful if the tool path stopped short of including all the elements of the part. You can examine the elements that were included and figure out where the problem is (usually, either a gap in the tool path, or a poorly designed intersection).
Check for collisions
Check the tool path for locations where the nozzle may move over an area where it can collide with pieces of already machined material. Areas of potential collision are highlighted in yellow.
Draw blue arrows that show the direction of the abrasive jet machining head. Right-click for options to control the drawing speed.
Show endpoint dots in the image
Use Zoom Cursor in drawing (left click zooms in, right click zooms out)
Zoom Window (click and drag to specify a window to zoom in on)
Pan (click and drag in preview window to pan the drawing)
Zoom Extents (fit all drawing elements in the preview window)
You should not be using the Custom tool path options on a regular basis. These are designed to be used for exceptional and rare situations. If you need to regularly create your tool paths by setting these options, then you are probably doing more work than necessary. Refer to the other topics and training videos listed at the end of this topic to better understand how tool paths work, and you'll save considerable time and effort.
Important: It is typically unnecessary to use the custom tool path options except for very rare and special applications (maybe 1 application in 10,000). You should be able to generate a tool path with the automatic settings and do so using only 1 to 5 mouse clicks. If you are doing more work than that, it is very likely that you are wasting time. Email Technical Support with your files for help in making this process more streamlined. The following are some tips you may find useful:
- When drawing your tool paths in the LAYOUT editor, always draw your leads so that they will cause the tool offset to be to the LEFT of the cutting path.
- If you find that the tool offset gets placed to the wrong side of the path, then remember to:
- Point the lead-in in the direction you want the jet to go.
- If it is already pointing in the direction you wish to go, then perhaps you need to swap your traverse such that your lead out becomes the lead in, and the lead in becomes the lead out.
- If you find that the Generate Path function is constantly stopping at intersections and asking you which way to go, then consider the following:
- Avoid intersections. Instead of having three or more entities that meet at a common point (a white dot), have them overlap without sharing a common point. For example, use two entities that overlap in a cross instead of 4 entities that share a common point.
- Make sure to run “Clean” on the drawing to remove duplicate and overlapping entities. Otherwise, these may be interpreted as intersections.
After following the above advice, contact Technical Support if you are still unable to accomplish your tool path automatically. It may be worthwhile using the custom options.
1) Right-click on the Path button.
2) Choose Custom tool path options from the menu.
Select this option from the right-click menu
3) A dialog appears offering options for creating the tool path.
Use this dialog to set the options for generating your tool path
Kerf compensation
There are three choices for offsetting the path to compensate for the kerf of the abrasivejet:
- Offset all to Left of path
The tool path is offset by the kerf amount to the left of the tool path. (Left and right are defined as to the left or right relative to the current direction of the tool path.)- Offset all to Right of path
The tool path is always offset to the right of the tool path.- Ask me at each opportunity
LAYOUT will stop whenever there's a chance that the offset could change (typically after a traverse line) and ask you to decide which side of the tool path the offset should be on.
When drawing a part, try to keep the offset always on the same side. This will keep the offset consistent, and make generating the tool path much faster.
Definition of a connected point
This number defines how closely two points need to be to each other for Order to consider them connected. The default setting assumes that any two points that are closer than 1/1000th of an inch (0.001 in.) apart should be considered connected.
This option is mostly useful when importing a DXF or DWG drawing from another program. Some CAD programs will not automatically connect points that are very close to each other, even though they appear to be connected. If the drawing has been imported, this value may need to be increased to make sure that points that look connected are connected.
The snap entities in LAYOUT make it easy to ensure that entities are connected. If the part was drawn entirely using LAYOUT, this number doesn't normally need to be adjusted.
The size of this number may need reducing if you are drawing a part with a lot of fine detail, where lines can be very close together without touching.
If a number that is too big for "Definition of a connected point" is entered, you may discover that the AutoPath stops and asks which way to go at intersections too often, and in areas you would not expect. This is because entities that are not really connected are considered to be connected.If you enter in a number that is too small, you may discover that the tool path will stop prematurely, as it will not be able to "spark" across tiny gaps, and will therefore think it has reached the end of the tool path.
Remove redundant dots
When this option is checked, endpoints that are not needed are removed from the tool path. In most cases, this is what you want. Sometimes, though, you may want to keep and endpoint to use as a reference for further manipulation in the 3-D Path Editor.
At intersection of Cutting Elements
This controls the behavior whenever two or more cutting elements (elements with a Quality other than traverse) meet. Choose either to have the computer decide which way to go, or ask it to stop and ask the direction to take.
When arriving at an intersection where the tool path could go multiple directions, LAYOUT uses the following logic to decide which way to go:
- LAYOUT takes the least sharp (or most tangent) path to the path it is on. (Much like if you were driving your car really fast and came up to a fork in the road, you probably would want to take the road that requires you to turn the least.)
- LAYOUT takes the path that it has not already taken.
At intersection of Traverses
Whenever two (or more) traverses intersect, this option controls what LAYOUT does. Choose to either have the computer decide which way to go, or ask it to stop and ask the direction to take.
The computer will use the same logic as it does for cutting element, as described in the previous paragraph.
Tool Path will be saved as a separate tool path file named:
Generating the tool path creates a file for a drawing that is used by MAKE. In most cases, you want this OMX file to have the same name as the part file (that is, if the part file is called PLATE.DXF you want the OMX file to be named PLATE.OMX).
In some cases, however, you may want to create more than one OMX file for the same drawing. Perhaps you'd be interested in trying different offsets for the part, for example.
Click on the Change button to bring up a standard Windows file save dialog. This dialog lets you choose a location and a name for the file.
4. Click to begin generating the tool path.
Clicking returns to the main drawing screen without generating the tool path.
5. Click on (or near) the start of the tool path. LAYOUT begins creating the tool path.
The cursor changes to remind you to click on the start of the tool path.
Click on the start of the tool path
6. If you specified LAYOUT should ask you about kerf compensation, a dialog appears at each intersection.
The offset is always specified as though you were standing on the tool path looking at the part.
After you select the offset, click on Continue to continue ordering the path.
Choose the side you want the offset to be on
7. If the custom options are set to have LAYOUT stop and ask when it reaches an intersection, LAYOUT will do so. When LAYOUT reaches a line intersection, the entity to continue the tool path must be specified.
When LAYOUT reaches an intersection, it will stop, zoom in on the intersection and highlight in yellow the possible ways that it can go.
Click on the yellow segment that the tool path should follow. A red line indicates that the tool path has already been along that entity.
Choose the direction for the tool path
There are three directions you could go in this example. The tool path can follow the circle either clockwise or counterclockwise, and there is also the lead-out--if the lead-out is chosen, the circle will not be cut.
8. When the tool path is complete, a dialog appears with a preview.
The tool path preview
Use this option to view tool paths for drawings that already have OMX files. The OMX file must be stored in the same location as the drawing file (this is the default location when the tool path is created) and have the same name as the drawing except with the .OMX file extension.
After selecting this option, a preview dialog appears.
Related topic