|
This section reveals all the essential points to take while running the machine, for complete 5XM setup, please follow our separate Setup Guide. |
Axis Directions and Coordinates System
Set-to-Zero Routine
|
This aligns reference to your machine space and 3D-model space. Now that you have BC Homing Script ready you can complete aligning machine axis to the 3D-model coordinate system. Option 1 (quick and dirty method) delivers a much faster process and might be an optimal choice when producing one small part. Option 2 (proper method) provides greater precision for mass production or when working on a large part over a number of days. |
Option 1: Set Zero to Stock
- Run B and C Homing Script in Mach3 and set B, C axis to zero.
- Jog the machine to any corner of the stock and type in Mach3 Input window to set the position to zero: G92 X0 Y0 Z0
- The chosen corner of the stock should be at zero coordinates in 3D modelling space.
Now XYZ coordinates are 0,0,0 in machine space and in the 3D-model at the same corner of the stock.
Option 2: Set-to-Zero Sensors (then offset to stock, recommended)
- Run B and C homing script to set B, C axis to zero.
- Home XYZ to their sensors by typing in Mach3 Input window: G28.1 X0 Y0 Z0
- Set these coordinates as zero by typing: G92 X0 Y0 Z0
Example on how to bring X-axis to its sensor and to set this position to zero:
- Zero coordinates are now set in the upper left corner of the machine.
- Stock to be placed approximately in the centre of working space, measure XYZ coordinates from zero point to either corner of the stock (top left) and input those three coordinates in your drawing space.
Example:
Now stock in digital 3D modelling space is placed exactly as in the physical space inside of the machine.
|
Useful tips prior to the operation on 5XM 1. How to check on the clearance for our Z-position? You might have noticed that the lower edge of the cube is significantly close to our vice. While this could lead to a crucial outcome (i.e. tool running into the vice by accident), we have come up with a solution for this particular case. This technique is fundamental as you will be able to predict whether your tool is likely to collide with the nearest object.
Once we extract the G-code for an individual roughing strategy, load it in Mach3. In Diagnostics Alt7 tab you will find Program Limits, which essentially gives you the lowest and highest points for all 5-axis. This will tell you how to manage your clearance area. For example, we have loaded the G-code for the left side of the cube and from the Program Limits, you can see that the tool won't go below -190.163. You can check this by jogging the tool towards our given coordinate and revise the clearance between the tool and the vice accordingly.
2. Set-to-Zero Routine: Be aware of the option that you're implementing. You should be extra cautious with Set-to-Zero Option 1. and try to use Option 2. unless you intend to complete the whole machining operation in one sitting ONLY. This option is known to be somewhat risky as you run a chance to lose your initial reference point, hence the tool might go elsewhere but the initial reference position. This usually happens as Option 1. provides only fast operation, which doesn't involve moving your stock off the vice. |
Post-Processor Installation
|
Before generating G-code, we need to make sure Fusion360 recognises 5axismaker for CNC milling. Each CAM package requires a post-processor made specifically for 5XM to take full advantage of 5-axis capability. Download the latest 5axismaker post for Fusion360 by visiting Autodesk Post Library. For all the steps on how to install a Personal (local) Post Processor in Fusion 360 CAM please follow this link. |
Run G-code: How to Post-Process
Post-process all 5 sides as 5 separate text files. To obtain G-code right click on the chosen toolpath and select Post Process, where an additional window will appear.
Make sure that you select 5axismaker in the Post Process window, setup the Configuration Folder and Output Folder where the G-code will be stored. In Program Settings below you specify the name of the file, from our example, we have selected the very first roughing strategy, i.e. top side.
Once you click Post button you will receive G-code in a Text Format, this is how your G-code will look like:
After obtaining the code, setup Mach3 (or Mach4) and load your G-code.
