Machine Operation
There are many steps to running a gcode file, please read carefully and follow all of the instructions. If you are ever unsure of something, please ask a staff member. Please budget at least 30 minutes (not including spindle warmup) for setup before you are able to run your code, even more if it is your first time.
Machine Startup
Step 1:
Switch the MAIN DISCONNECT to ON located near the back-right of the machine. The lights in the machine will turn on.
Step 2:
Release the E-Stop button by twisting it counter-clockwise until it pops up.
Step 3:
Press the physical RESET button which will then light up.
Step 5:
Click the RESET button on the screen.
Step 6:
Reference the axes by clicking REF Z first then REF X and REF Y. Once finished they should show up green.
Spindle Warmup
If it has been more than 4 days since the machine was last used, you will need to run the spindle warm up.
You can find the file if you go to the File tab, and select SpindleWarmUp.nc so it is highlighted blue. Then click the LOAD G-CODE button.
From the Main tab, click CYCLE START to begin the spindle warm up code.
Ensure the door is closed before starting.
We can see the code waits 200 seconds at each of the following spindle speeds: 525, 1000, 2500, 5000, 7500, 10000 RPM. If you are really pressed for time and not using a very high spindle speed, you may cancel the job early once you have surpassed the highest spindle speed you will be using.
You can see the current line of gcode that the machine is on is highlighted orange.
In this example, the spindle is currently spinning at 1000 RPM.
Loading Tools
Components:
Tool Holder (chuck)
Collet
Tool/ Bit
Wrench *Only use one pictured*
Note: The collet hole diameter should be the same size as the tool bit shank (smooth non sharp portion).
Step 1:
Place Tool Holder into tightening fixture on tool cart next Milling machine.
Note: Tool holder can be placed vertical or horizontal
Step 2:
Unscrew collet nut and place collet into nut. Orient the collet at an angle to snap into place.
Step 3:
Place Tool/Bit into collet and collet nut.
Step 4:
Hand tighten collet nut and bit onto tool holder.
*Make sure collet is flush with collet nut before tightening*
Step 5:
Then use wrench supplied to tighten.
*Do not over tighten*
Step 6:
When loading tool holder into spindle be careful of hand placement.
Grab tool holder below metal groove shown above.
Step 7:
Press the Clamp button on the left side of the ATC to load tool holder into spindle.
Firmly hold the tool holder and ensure it is loaded into spindle before releasing grip.
Step 8:
Assigning Tools to ATC (Automatic Tool Changer)
Click the ATC tab, then using the "Tray FWD" or "Tray REV" button move the ATC to an empty tray slot.
Step 9:
Type the number you would like to assign to the tool into both the T_M06 G43 on the bottom right hand corner of the screen and to the top left where it says "Insert"
Example:
T1 M06 G43
1 Insert
Once both sections indicate the same number press the "T_M6 G43" button
*This will let the ATC know what tool is currently in the spindle*
Step 10:
Now click the "Insert" button making sure the T_M6 G43 number still matches. An Asterisk should appear in the selected tray spot.
*If an asterisk does not appear and it shows the number in the selected tray instead, Do not move on to the next step*
Follow the steps below then repeat steps 9 and 10 from the beginning again.
Press "Remove" on the top right side of the screen making sure the number associated with tool you are loading is shown next to the Remove section. A prompt will be shown asking to remove the tool from spindle and the number should disappear from the selected tray.
*You do not need to remove the tool from the spindle*
Step 10:
Click "Store Current Tool" this will place the tool in the ATC in the assigned Tray.
T_M6 G43 reads T0 since there is no tool in the spindle now.
Note: If there are multiple tools in the ATC you can select the tool you would like by typing the number desired in the T_M6 G43 command.
Setting Tool Offsets
Setting Tool Offset using the Zero Setting Gauge
Step 1:
Place Zero Setting Gauge on vise.
*ZSG - Zero Setting Gauge*
Step 2:
First, you need to touch off the spindle with no tool onto the ZSG.
Slowly lower the spindle over the ZSG as shown above.
*Adjust rate of speed to x10*
Step 3:
Once the ZSG hits 0, continue to lower the Z axis to until the dial reaches 0 once more.
*Adjust rate of speed to x1*
Step 4:
Once you are at 0 on the ZSG for the second time. You will press Zero Z button. You should see 0.00 in the Z axis for the G54 work offset.
Step 5:
Now you can raise the spindle and fetch a tool from ATC
*Make sure vise is not below spindle or ATC*
Step 6:
Position tool above ZSG making sure the Z axis is clear first.
*When using the jog dial always check which axis and rate of movement is selected prior to moving*
Step 7:
Slowly lower the Z axis until the dial on the ZSG starts to move.
*Adjust the rate of movement to x10*
Step 8:
Once the ZSG hits 0, continue to lower the Z axis to until the dial reaches 0 once more.
*Adjust rate of speed to x1*
Step 9:
Select Offsets tab. This will show the tools loaded in the machine including the tool length offsets shown on the right hand side
Adding a new Tool:
If your tool is a Tormach tool, input the last five numbers on the tool container located on the black cart.
Step 10:
Once you've selected the correct tool above. Select "Touch Z" or Press "Zero Z" to set the Tool length offset based off the ZSG.
Step 11:
Check Zero Z, it should be 0.00 and check the corresponding Tool Length section, as it should have changed as well.
Step 12:
Slowly raise the Z axis checking that you are moving in the Positive direction to remove the ZSG from the vise.
*Refer to jog dial for + and - indicators*
Material Fixturing
We will cover how to fixture your (relatively) square workpiece in a machinists vise. Larger workpieces may need to be fixtured with t-slot clamps and non square workpieces may need soft jaws for the vise to be clamped well. Please ask a staff member if you have a need for either of those situations.
Fixturing a square workpiece in a vise
Fixturing a workpiece using t-slot clamps
Fixturing a round workpiece in a vise using soft jaws
Step 1:
Select a pair of parallels that are an appropriate height for your workpiece. They are kept in the top drawer of the Tormach's tool chest.
Parallels are thin, precisely machined rectangular pieces that are used to keep your workpiece held parallel above the bottom of the vise. This allows you to machine the top of the workpiece without cutting into the vise jaws or to drill all the way through the piece without damaging the vise.
Step 2:
Place your parallels in the vise against the side of the vise jaws (the sides that will clamp onto your part).
Step 3:
Put the handle on the vise. It may be on the tool chest or next to the keyboard.
Step 4:
Put your workpiece on the parallels in between the jaws.
Step 5:
Slightly tighten (not too tight) your workpiece in the jaws by turning the handle so it can no longer slide around. Then use a dead blow hammer to give it some firm taps while tightening the handle to be very tight. Check that neither the workpiece or the parallels can move. If the parallels are still able to slide around, loosen the vise and try again.
This process ensures that your workpiece is really flat on the parallels because tightening can sometimes cause it to slightly tilt up on one side.
Congratulations, you've clamped your material in tightly and you're ready to start locating your workpiece origin.
Zeroing Your Material
Zeroing the X and Y axes
We will cover how to zero the x and y axes with an edge finder. If you are very comfortable with this method and want to try using a probe, let a staff member know.
Step 1:
Locate the edge finder in the tool chest. It may be in a tool holder already.
An edge finder is a tool with a small cylindrical body attached at the end of a larger cylindrical body. The small cylinder portion is attached to the large cylinder by a spring that allows it to spin off center of the small cylinder. This makes it look like it wobbles and gives us a visible difference in behavior when it begins to touch the side of a workpiece. Our tool has a center finder (pointed side) on the other end.
Step 2:
If the tool is not already in a tool holder, follow the Loading Tools section above to put it in the appropriate size collet and into the tool holder. You may need to align the center finder side to get it to slide into the collet. Then load it into the spindle. Ensure any tools in the spindle are back in the ATC.
Step 3:
Using the jog controller, jog the edge finder to the side of the workpiece where you want your x axis to be zeroed. The small cylinder should be slightly lower than the top of your workpiece.
Ensure your small cylinder is sitting off center.
Step 4:
On the controller, type 750 into the spindle speed box and click Enter. It is important that you see the desired RPM there before you click the FWD button. When you the number without the cursor, click FWD to start the spindle.
You should see the small cylinder of the edge finder look like its wobbling.
Step 5:
Using the jog controller, approach the edge of the workpiece slowly in the x direction. You should see the small cylinder stop wobbling and start spinning more centered as it begins touching the workpiece.
Step 6:
At this point move very slowly, using the finest jog rate. The small cylinder will get very aligned with the large cylinder and then once it's actually tangent to the edge it will pop to the side and you will want to stop immediately.
I recommend looking through the side windows for the x axis because it is difficult to see it pop from the front.
The small cylinder is aligned with the large cylinder meaning that we are almost tangent with the edge.
The small cylinder has just popped to the side indicating that it is tangent to the workpiece edge. Stop jogging immediately.
Even though we've found the location where the tool is tangent with the workpiece, we don't want to zero the x axis here because this is not the center of the spindle. However since we know the diameter of the small cylinder is 0.2 inches, we just need to move towards the workpiece 0.1 inch and zero the x axis there.
Step 7:
Without moving in z, on the jog controller, change the axis to the z axis and move above the part. Stop a place where the dial is on 0.
Step 8:
On the jog controller, change the axis back to x and ensure that the step rate is at X10 (.01"). Turn the dial one full rotation to arrive back at zero. Since I found the edge on the left side of the part I will move in the + direction.
This will move us 0.1 inches over the workpiece. Visually verify that the center of the edge finder is over the edge of our workpiece.
This looks like we have found the correct edge location.
Step 9:
On the control panel, click the Zero X button to set that location as zero in the G54 work coordinate system. The X POS IN G54 should change to 0.000.
Step 10:
Turn off the spindle, move the small cylinder off center again and turn it back on. Repeat the above steps to zero the y axis.
Zeroing the Z axis
When zeroing the Z axis you will load a tool into the spindle and touch it off to the top of your work piece. There are a few ways to accomplish this, the method outlined in this tutorial will be using small piece of paper on top of the workpiece and slowly lower the tool onto the paper until you feel a drag or resistance when you try to pull on the piece of paper.
*Adjust Step rate to x1 for Z axis movements*
Step 1:
Load tool into spindle from ATC then tear off small piece of paper and place it roughly in the center of your workpiece
Slowly lower your tool just above the piece of paper not touching
*Always check the jog dial to know which axis you are moving and which step rate is active before moving*
Step 2:
Once the tool is just above the paper make sure the step rate is at x10 and the Z axis is selected. Then move the jog dial one notch at a time until the tool makes contact with the paper
Step 3:
Adjust the step rate to x1 with the Z axis selected. Then move the jog dial one notch at a time while moving the paper back and forth. Stop moving the jog dial once you feel resistance on the paper.
Step 4:
Once you feel resistance or the paper start to drag. Select the Z zero button in the Path pilot controller.
After Z zero is selected the numbers to the right should be zeroed out like shown above.
Now your Z axis is zeroed and you are ready for the next step!
Running an Air Pass
Before running the Gcode, an Air Pass is run 2 inches above the part to ensure that the Gcode is running as intended on the machine. This is to catch any errors prior to running the Gcode on your part.
Step 1:
Using the jog dial. move the spindle 2 inches above the Z Zero and then select Z Zero to make this location the new Z Zero for the Z axis.
Step 2:
The next step is to load your Gcode.
You will need to plug in your USB to the controller then select file and double click the corresponding gcode you would like to load.
Gcode loaded above
Important things to know before running your Gcode
Cycle start: This will run whatever Gcode that is selected or loaded. *If single block is selected, you will have to press Cycle Start for every line of code*
Feed Hold: This is a pause in case something happens that isn't critical or you want view your part. Pauses the job where you are and it's possible to continue. You will have your finger over feed hold and Cycle start through out the job.
Emergency Stop: This is the something has gone terribly wrong button and you need to stop everything. Resets the machine.
Single Block: In order to use Single Block you need to select it prior to selecting Cycle Start. This will allow you to run one line of code at a time giving you more control if something goes wrong and the opportunity to see where something goes wrong if it does.
Step 3:
Select Single Block - the green circle will appear on the top right corner if it's active. YOU MUST USE SINGLE BLOCK ON YOUR AIR PASS.
Additionally, the MAX VEL dial must be below 15%.
Step 4:
Now you are ready to run your Gcode with a 2 inch safety buffer
Hover over Feed Hold and press Cycle start. This will start your first line of code. You will have to press cycle start after each line to continue to job until it reaches the end of the code.
Step 5:
Once the air pass is completed and no errors remain. Remove the 2 inch safety buffer by using the jog dial and manually moving the Z axis until the Z axis reads zero. Once the Z axis reads 0.00 manually write in 2.00 into the Z Zero. This will remove the 2 inch buffer.
Running Your Gcode
Running your Gcode is the very last step in the setup. Please make sure the air pass goes through without any errors before running the Gcode without the 2 inch safety buffer.
Important things to know before running your Gcode
Cycle start: This will run whatever Gcode that is selected or loaded. *If single block is selected, you will have to press Cycle Start for every line of code*
Feed Hold: This is a pause in case something happens that isn't critical or you want view your part. Pauses the job where you are and it's possible to continue. You will have your finger over feed hold and Cycle start through out the job.
Emergency Stop: This is the something has gone terribly wrong button and you need to stop everything. Resets the machine.
Single Block: In order to use Single Block you need to select it prior to selecting Cycle Start. This will allow you to run one line of code at a time giving you more control if something goes wrong and the opportunity to see where something goes wrong if it does.
Step 1:
The next step is to load your Gcode.
You will need to plug in your USB to the controller then select file and double click the corresponding gcode you would like to load.
Gcode loaded above
Step 2:
Select Single Block - the green circle will appear on the top right corner if it's active. YOU MUST USE SINGLE BLOCK ON YOUR FIRST RUN.
Additionally, the MAX VEL dial must be below 15%.
Step 3:
*Keep in mind there is no 2 inch safety buffer, the tool will go into your part*
Hover over Feed Hold and press Cycle start. This will start your first line of code. You will have to press cycle start after each line to continue to job until it reaches the end of the code.
Cleaning Up
Parallels: clean and free of debris/chips placed back in box
Vise: Jaws should be clean and free of debris. Clean off chips from top of vise
Table: Use air to blow chips on the table. Metal chips are sharp!! Keep one door closed and your body behind that door to prevent any chips from blowing back at you. There must be a tool in the spindle when using the compressed air to keep chips from blowing up there.
Oil: Please wipe down the vise and table with WD-40.
Machine Shutdown
Step 1:
Click EXIT on the screen in the bottom right corner.
Step 2:
A message will pop up telling you to press the E-stop button. Do so then click OK.
Step 3:
Turn the MAIN DISCONNECT to OFF.