Sodick SL400G Wire-EDM
The wire-edm cuts material with a thin brass wire. It does so using a process called spark erosion. This means that your workpiece has to be conductive. While it's one of the slower machines in the lab (feedrates are on the order of .1 in/min), it's great for making super-precise parts out of difficult to machine materials like hardened steel.
Here's an example of an application it's perfectly suited for - custom tool and die for stamping out plastic Lego-GIK
This is the manual for the wire-edm.
- Set your condition number:
- Before you do anything with the machine you should make sure that it's using the right settings for the diameter of wire that's installed.
- By default when it turns on, it's expecting 0.010" wire.
- To change this, go to Edit, select the file named "Cond" (this should already be loaded in memory). Find the condition number that has the right settings (a 6 mil wire should have a WK value of 015). Enter this number (e.g., 0006) in the yellow Cond. Num. entry box. Press ENT.
- Installing the wire. You'll need to do this if you change wire diameter or if the wire breaks.
- Often this is easier if you turn off the backtension on the spool. You can do this by going to Manage --> Parameter --> User 1 and then change "Backtension Select" to 1.
- Then, just string the wire through the path depicted in the below image.
- You'll need to move the "AWT pipe" down to thread it through the upper guides. Do this by holding the "AWT Free" button (to the right of the wire path) while sliding the pipe downward.
- Now thread the wire through the top of the pipe and move the pipe back into position.
- It should now be possible for the machine to thread itself. Hit the "Thread" button and hope for the best.
- Design your part. Ensure you leave radiuses or dogbones in the corners equal to or greater than the kerf of the wire. (A good rule of thumb is wire_diameter*1.5 but you can also check by doing a "condition search".)
- It also makes life easier to add a point wherever you want to start your toolpath.
Here, I pre-cut the cyan lines on the waterjet.
- Fixture and setup the part:
- Clamp your part.
- Set your z-height. Cut the wire --> Position the head over the stock --> Move the head down until it just touches a 4 mil spacer (Use MRF 2 to move slowly) --> Manual --> Coord. Set --> Select Z --> hit ENT.
- Pickup the edge of the stock. Thread the wire --> Manual --> Approach Face --> x,(-),coordinate_set=on,ABS --> ENT
- Make the G-Code:
- If the USB is in the machine eject it by clickin on the "EXT Memory" button at the very top of the screen.
- Drag your .dxf file into the UTY folder of the Sodick USB stick. Make sure your filename is eight characters or less (not including the extension) otherwise HeartNC won't see it.
- Go to IQ --> File and drag the file from the EXT Memory into "IntelligentQ3vic"
- Go to IQ --> HeartNC and click File --> Open and select your file.
- Select Wire Cut Defs and choose Die or Punch based on what you're cutting.
- Hit Gen NC Data to generate the G code.
- Check the G-Code:
- It's important to check the G-Code to make sure the machine is happy with your file and can get in all the corners.
- First, make sure the interference check is enabled. Go to Edit --> Graphic --> Setting --> Setting --> Detail (tab) and change the "Interference Check" parameter to 1.
- Press carriage return and then okay to apply the change.
- Load in the G-code that you generated.
- Now, go press Draw. If there's no error message then you're good to go.
- If you got an error message, and think you're correct, you can have the software automatically ignore it by changing the interference check option to 0.
- Make sure to press "Save" before running the job. This will ensure that you can see the progress as it runs.
- Run the job:
- If you're part is less than a few inches thick it's good to keep the doors at half-height. This is done by going to Manual --> MDI --> type M36 --> press ENT.
- Now we're ready to go.... Go to Run.
- Press "Home" on the keyboard to go to the top of the g-code.
- Press ENT to start the job.
Things to be wary of:
- Power Failures
- It's not uncommon for the machine to experience a "power failure." It usually happens just as it's about to energize the wire at the start of a job. When it happens, to fix it go over to the breaker on the other side of the Hurco and flip the bottom-right-most breaker back and forth to reset it. Wait a minute or two and then try hitting the "ENT" button. If all goes well the machine will regain power, move the axes back to where they should be, and continue the job. In most cases the wire will be somewhat mangled from the sudden stop though so I tend to stop the job, rethread the wire, and then restart it where it left off.
- Coordinate system changes.
- When you're cutting a die (especially ones with multiple internal cuts), the g-code will switch between coordinate systems (G54 and G59, for example). It's therefore good practice to zero all coordinate systems (you can just check to the box that says "all cord. sys. set").
- Small slugs in the flush cup.
- If your job produces small slugs, be wary that they can often make their way into the flush cup and cause unnecessary short circuits. The fix is to simply stop the job, open the flush cup, remove the debris, and then resume the job from where it left off.
Tips and Tricks:
- Optimizing the order of the cuts.
- You can choose the order in which rough and finish cuts are made with the "Machining Process" selection when you go to generate NC data in HeartNC. The selections aren't very self-explanitory so refer to this document for what they mean. For die cutting I like to change it to "DIE-cut in advance fine"; this should minimize the number of times it needs to cut wire and rethread.
- Close the loop! - Measure your parts
- If you really want to get a part within a tight tolerance you should use the wire-EDM to measure your part before you remove it. You can, for example, check the diameter of holes with the "Hole Center" codeless interface. You can also check the width and angle of cutouts.
- Know your offsets
- The gcodes that HeartNC generates are easily modifiable if you find that the cut is smaller or wider than the default setting. The there should be a series of
Hxxxx = 0.xxxx; in the header. These are literally the wire offsets that the gcode will later refer too. If you need to open up a whole by 0.010", for example, just decrease the offset by 0.005."
- Take a screenshot
- You can take a screenshot the same way you do on any windows computer. Hit Print screen. Display the windows start panel by hitting ctrl + shift + alt + s. Launch MS paint (in Accessories). Ctl+V to paste the image, and then save it onto the USB drive.
G-Codes To Know:
A full list of G-Codes for the machine can be found here but these are a few of the most useful:
- M36 sets the door height to half height (useful if you're not burning tall parts). It's recommended to enter this if you're doing a thin (less than a few inches tall) part so that you can better see the action.
- G54-->G59 change your coordinate system
- G92X__Y__Z__ sets the current coordinate system to the given coordinates
- G26RA___ rotates the part by ___ degrees. (G126/G127 do this too and is used by the auto-tilt correction) ** This may modify your x,y