Skip to main content

v2.3

Minor Versionm

by Kenny Davis Jr

Parts

No parts specified.

  1. Creating a rectangle on top will allow us to easily create a facing feature Begin by clicking on the topmost surface, and create a sketch Then, draw a rectangle around the top, and make it 6 x 4.5". Centering is optional (use relationships)
    • Creating a rectangle on top will allow us to easily create a facing feature

    • Begin by clicking on the topmost surface, and create a sketch

    • Then, draw a rectangle around the top, and make it 6 x 4.5". Centering is optional (use relationships)

    • The last photo is a finished view.

  2. This is where we will begin our CAM. CAM stands for computer-aided design, and thus a tool integrated right into Fusion 360 that allows us to create G-code. Over in the left toolbar where it says "Design," drop down the menu and select "Manufacture." Next, we need to create a new setup. Click the new setup button as shown by the orange rectangle, or taskbar.
    • This is where we will begin our CAM. CAM stands for computer-aided design, and thus a tool integrated right into Fusion 360 that allows us to create G-code.

    • Over in the left toolbar where it says "Design," drop down the menu and select "Manufacture."

    • Next, we need to create a new setup. Click the new setup button as shown by the orange rectangle, or taskbar.

    • For more complicated parts with a top and bottom, multiple setups can be used. But we will only have one for this guide.

    • After selecting the new setup button, it will bring up a menu for setting orientation and stock size.

  3. For orientation, we always keep the same model. The positive Z-axis is the spindle. The X and Y-axis are up to the user, but the red rectangle shows how both are orientated. The first option for most operations is the "Stock Point." Always be sure to select the top middle point. * NOTE - sometimes while doing the setup, this can jump on you. If it ever does just be sure to select "Stock Point," and choose the top middle again.
    • For orientation, we always keep the same model. The positive Z-axis is the spindle. The X and Y-axis are up to the user, but the red rectangle shows how both are orientated.

    • The first option for most operations is the "Stock Point." Always be sure to select the top middle point.

    • * NOTE - sometimes while doing the setup, this can jump on you. If it ever does just be sure to select "Stock Point," and choose the top middle again.

    • In the menu, navigate to the "Work Coordinate System" and drop down the menu for "Orientation." In this dropdown, select the "Select Z axis/plane & X-axis" option.

    • Now on the menu, the selection for the Z-axis should be highlighted. Navigate through the part origins, and select the axis that is "coming out of the part." (In the picture shown, it was the Y-axis)

    • For the X-axis, select the best axis option for the particular part. In our case, it is how we orient the part.

    • Lastly, just double-check the "Stock Point" and validate it is in the top middle.

  4. For setting the stock size, follow all the steps here. But the actual length, width, and thickness can be varied to particular needs and what is available. On the pop-up bar select "stock," and navigate down to "mode." Change this to "Fixed Box Size." Type in the X and Y dimensions available, or copy 6 x 4.5" For the Z-axis, drop down the menu by "Model Position" and select "Offset from Bottom (-Z)." Then make sure this offset is 0". My thickness is .75"
    • For setting the stock size, follow all the steps here. But the actual length, width, and thickness can be varied to particular needs and what is available.

    • On the pop-up bar select "stock," and navigate down to "mode." Change this to "Fixed Box Size."

    • Type in the X and Y dimensions available, or copy 6 x 4.5" For the Z-axis, drop down the menu by "Model Position" and select "Offset from Bottom (-Z)." Then make sure this offset is 0". My thickness is .75"

    • Lastly just change te view around the model, making sure the stock completely covers the part. Shown in the green is the top, which was my check.

  5. The Face operation will cut-away material to bring the top material down closer to the part. Select the "Face" operation by dropping down the menu for "2D," and electing "Face." By tool, click "select." Navigate to the EZ_Router_Wood library and select the face tool "30 - 1.5 Diameter."
    • The Face operation will cut-away material to bring the top material down closer to the part.

    • Select the "Face" operation by dropping down the menu for "2D," and electing "Face."

    • By tool, click "select." Navigate to the EZ_Router_Wood library and select the face tool "30 - 1.5 Diameter."

    • The facing tool usually has a bigger base at the bottom as shown in the photo.

    • Going in line with the next option, geometry. Simply select the rectangle we drew in step 1, and the words will change to "chain."

  6. Next in the "Heights" tab,  there is nothing we need to change but verify. If all the values are shown as in the red rectangle, you are golden. Bottom Height - The lowest height the operation will mill. Top Height - usually just the top of the model. Feed Height - the height at which the spindles starts to rotate, and the height linking moves are made. Clearance Height - should always be above all features on a model. Retract Height - the height at which the machine will retract the tool. On the passes tab, select the "Multiple Depths" option, and set the "Maximum Stepdown" to .125" and click "OK" at the bottom.
    • Next in the "Heights" tab, there is nothing we need to change but verify. If all the values are shown as in the red rectangle, you are golden.

    • Bottom Height - The lowest height the operation will mill. Top Height - usually just the top of the model. Feed Height - the height at which the spindles starts to rotate, and the height linking moves are made. Clearance Height - should always be above all features on a model. Retract Height - the height at which the machine will retract the tool.

    • On the passes tab, select the "Multiple Depths" option, and set the "Maximum Stepdown" to .125" and click "OK" at the bottom.

    • After the simulation should be shown after clicking on the face operation in the structure tree to the left.

  7. Right-click the operation you want to simulate and select "Simulate." When the menu pops-up, be sure to select the "stock" option. This will allow everything to be seen more clearly. On the bottom, a simulation menu will be available. By selecting the play, you can see the whole simulation. There is also a fast-forward, fast-reverse, and skip to end buttons.
    • Right-click the operation you want to simulate and select "Simulate."

    • When the menu pops-up, be sure to select the "stock" option. This will allow everything to be seen more clearly.

    • On the bottom, a simulation menu will be available. By selecting the play, you can see the whole simulation. There is also a fast-forward, fast-reverse, and skip to end buttons.

    • The sliding bar is the speed. It can be adjusted to however fast or slow you would like.

    • When finished click "Close" on the bottom of the pop-up box.

  8. 3D Adaptive clearing will cut away a lot of material at once, but will not me the finishing touch. Go to the 3D drop-down menu, and select "Adaptive clearing." For the tool, we are going to use a 1/2" end mill. At the machine, we will use the anama tool but simply select the #1 1/2 diameter end mill.
    • 3D Adaptive clearing will cut away a lot of material at once, but will not me the finishing touch.

    • Go to the 3D drop-down menu, and select "Adaptive clearing."

    • For the tool, we are going to use a 1/2" end mill. At the machine, we will use the anama tool but simply select the #1 1/2 diameter end mill.

    • In the geometries tab under "Machining Boundry" select "Bounding Box." This will bound all operations to a specific area.

  9. Next, go to the heights tab. Scroll down to the "Bottom Height" row and drop down the menu, selecting "Selection." Now select the lowest contour pocket (the breadboard cutout). In the passes tab, make sure "Stock to Leave" is checked. Set both values to .02". Stock to leave is essential for a fast, smooth finish. With the adaptive clearing, we are just getting rid of tons of material at once. Later on, we will come back and "polish" it.
    • Next, go to the heights tab. Scroll down to the "Bottom Height" row and drop down the menu, selecting "Selection." Now select the lowest contour pocket (the breadboard cutout).

    • In the passes tab, make sure "Stock to Leave" is checked. Set both values to .02".

    • Stock to leave is essential for a fast, smooth finish. With the adaptive clearing, we are just getting rid of tons of material at once. Later on, we will come back and "polish" it.

    • When finished, select "OK" and simulate to check for any errors.

  10. Select the "Horizontal" operation in the "3D" column. For this operation, we will be using the 1/8" anama tool. Select the # 4 1/8" flat end mill tool. For geometries, we will copy the same operation we completed for adaptive clearing. Change "machining boundary" to "Selection" and select the rectangle dawn in step one.
    • Select the "Horizontal" operation in the "3D" column.

    • For this operation, we will be using the 1/8" anama tool. Select the # 4 1/8" flat end mill tool.

    • For geometries, we will copy the same operation we completed for adaptive clearing. Change "machining boundary" to "Selection" and select the rectangle dawn in step one.

  11. As we did for adaptive clearing, in the "heights tab," in the "bottom height" row, drop down the menu and select "Selection." Then click the lowest pocket (the breadboard pocket). Now go to the passes tab, and click "smoothing." The value should be preset, don't change it. As stated earlier, now we are going to smooth all of the surfaces. This is different from adaptive because we are not taking a lot of material out, so we can use a smaller mill with less strength.
    • As we did for adaptive clearing, in the "heights tab," in the "bottom height" row, drop down the menu and select "Selection." Then click the lowest pocket (the breadboard pocket).

    • Now go to the passes tab, and click "smoothing." The value should be preset, don't change it.

    • As stated earlier, now we are going to smooth all of the surfaces. This is different from adaptive because we are not taking a lot of material out, so we can use a smaller mill with less strength.

    • When finished click "OK" and simulate the operation.

    • NOTE - To simulate all the operations, just right-click the setup, and select "simulate."

  12. Select the "Bore" operation under "2D." We will be using the same tool used in the previous operation. the #4 1/8" diameter end mill, in the EZ_Router_Wood folder. Next in the "Geometry" tab, simply just select the 4 holes on the outsides of the part. We are going to bore with a helix down these holes.
    • Select the "Bore" operation under "2D."

    • We will be using the same tool used in the previous operation. the #4 1/8" diameter end mill, in the EZ_Router_Wood folder.

    • Next in the "Geometry" tab, simply just select the 4 holes on the outsides of the part. We are going to bore with a helix down these holes.

  13. Nothing else needs to change, but verify the "bottom height" in the "Heights" tab is set to "Hole Bottom." Run the simulation to verify no errors. Remember it would be best to run the full simulation. If zooming into a hole, the helix is clearly visible.
    • Nothing else needs to change, but verify the "bottom height" in the "Heights" tab is set to "Hole Bottom."

    • Run the simulation to verify no errors. Remember it would be best to run the full simulation.

    • If zooming into a hole, the helix is clearly visible.

    • The helix is because the end mill is made for milling, not drilling. Therefore by creating a helix, it will "mill" down, and do what the bit is intended for.

  14. Select the "2D contour" operation in the "2D" tab. We will be using the same tool used in the previous operation. the #4 1/8" diameter end mill, in the EZ_Router_Wood folder. In the geometries tab, select the bottom-most outer contour. (The blue outline, by the green arrows).
    • Select the "2D contour" operation in the "2D" tab.

    • We will be using the same tool used in the previous operation. the #4 1/8" diameter end mill, in the EZ_Router_Wood folder.

    • In the geometries tab, select the bottom-most outer contour. (The blue outline, by the green arrows).

    • Remeber we are choosing th bottom-most countour because this operation will cut the part out.

  15. In the "Heights" tab, on the "Bottom Height" row, set the "from" to "model bottom," and offset -.01". We will barely cut into the table, just skimming it to make sure that part is completely cut out. Next in the passes tab, turn on "smoothing." Leave the preset value alone.
    • In the "Heights" tab, on the "Bottom Height" row, set the "from" to "model bottom," and offset -.01".

    • We will barely cut into the table, just skimming it to make sure that part is completely cut out.

    • Next in the passes tab, turn on "smoothing." Leave the preset value alone.

    • You can turn on multiple passes if you feel it needs it, but the cut is so small it almost unnecessary.

    • Lastly, simulate to check for errors.

  16. ALWAYS DO A FULL SIMULATION AND ADDRESS ALL ERRORS BEFORE CUTTING AT THE MACHINE As previously stated, right-click on the setup and simulate. Play the whole simulation through, looking for errors.
    • ALWAYS DO A FULL SIMULATION AND ADDRESS ALL ERRORS BEFORE CUTTING AT THE MACHINE

    • As previously stated, right-click on the setup and simulate.

    • Play the whole simulation through, looking for errors.

    • When finished the part should be cut out.

  17. Click the "Create NC" program. This will generate the G-code the EZ-router CNC machine. Create a unique 4-digit number for the "Name/number." Then put a comment for some clarity as to what the program is. Lastly, set the "Output Folder" to where you want the NC program to output, most likely a removable drive. When finished click "OK" and the G-code program has now been exported. The G-code commands the EZ-Router to follow a set of instructions.
    • Click the "Create NC" program. This will generate the G-code the EZ-router CNC machine.

    • Create a unique 4-digit number for the "Name/number." Then put a comment for some clarity as to what the program is. Lastly, set the "Output Folder" to where you want the NC program to output, most likely a removable drive.

    • When finished click "OK" and the G-code program has now been exported. The G-code commands the EZ-Router to follow a set of instructions.

Kenny Davis Jr

Member since: 11/14/2019

2,726 Reputation

23 Guides authored

Team

TW: Staff Member of TW: Staff

173 Members

284 Guides authored

0 Comments

Add Comment