Success CNC roughing a straight cut bevel gear. Gearotic + SheetCAM TNG
Posted: Sat Jun 02, 2018 1:46 pm
Hey Everybody. I'm Andrew. And in this post I'm going to ramble on about how you can CNC cut a straight cut bevel gear on a 3 axis machine with help from Gearotic and Sheetcam TNG.
Step 1 : Design your Bevel Gear in Gearotic. Its mostly about the tooth count and shaft angles at this point . Do yourself a favor and make the gear significantly wider than the finished gear you will be needing, as you will need the extra data further along for the machining process. As long as the tooth count and shaft angles are correct, the gear you need will be somewhere in there, within the extra long gear you just created.
Step 2 : Select your gear and go to the DFX output in Gearotic and spit out a 2D drawing of your gear. Use the side on view of this drawing as a guide to manually machine a gear blank out of whatever material it is that you desire to make your gear from. Make sure to center drill the gear blank or make your shaft bore. Just remember you will want some way of indicating where your center point is for setup later in the CNC. Also make sure you have a way of mounting this blank later on in your cnc mill. Usually the gear will need a shoulder on the backside anyway.
Step 3: In Gearotic, right click on your gear in the project tree and click "send selected to slicing module". Flip the gear using the perspective controls so you are looking at the gear from the back side. You do this as slicing starts from the bottom up, as would be needed for 3d printing. But we need the information in reverse, as cnc milling is generally done from top down. Next set your slice thickness. Keep in mind that the slice thickness you use now will also need to be your cutting depth for each pass on in your machining operation. Thinner slices will equal better resolution and less finish work on your gear later. But your CAD and program files will be much larger and your machining process will also be longer with very thin slices. My happy medium so far is .020 thickness. Go ahead and hit that slice button. Then you go down to the slice viewer slide bar, and have a look at how many slices you will need to form your gear. Make a note of what slice number that the outside contour starts to go back under the outside tip of the gear teeth. Any slice number past this will be no good as a milling tool cannot reach underneath the tip of the tooth and if these slices were programmed for milling, the machine would in turn mill off the majority of your outer tooth profile. Remember in step 1, when I said make your gear thicker than what you need? This is why. You need that thick gear design so you have a contour to follow all the way down to the root of the teeth. The last several passes of your machining operation your cutter will be "out in space" machining the tips of imaginary teeth as the real teeth ended long ago, but the cutter will be then coming back in and cutting metal out from the root area. Now you can select "0,0,0" option under "output slice" and click the "DFX Out" button.
Step 4: Go ahead and fire up SheetCam TNG! everybody's got sheetcam, right? Next Import your new sliced up gear drawing into Sheetcam. Make sure to select "Center Drawing on 0,0" when importing. This will automatically put the centre of your gear on x0,y0. Making everything way easier for setup and machining. Also For some reason, Gearotic puts loads of empty layers in its DFX output file. If you wanna be a rockstar, you can first use your favourite 2d CAD and delete all that extra crap before loading it into Sheetcam. You can also delete the slices that go back underneath the lower gear tip that I described in step 3. Now comes the really AWFUL NASTY TERRIBLE PART. You've gotta program a separate outside contour operation in Sheetcam for each slice, starting at slice 1 and going all the way down till the last slice before your contour starts to go underneath the outer tooth tips. ( if you didn't already delete them). IT IS SUPER IMPORTANT that you program each operation's depth of cut to the exact thickness that you made your slices in step 3. And that each successive slice's starting depth is exactly that of the previous slice's finish depth. If you don't do it right your gear will come out dis-proportioned or you'll break some stuff. Then go ahead and post your G-code with whatever post processor your mill unit can read.
Step 5: Mount your gear blank in your CNC mill. I clamp a 3 jaw to the mill table and grab onto the shoulder of the gear, of course with the bevel facing up toward the spindle. Zero everything up in the center of your blank, cross your fingers and hit the whatever it is you got for a go-go button. See what happens!
AFTERTHOUGHTS:
You may want to program a large endmill to make a few laps around the largest contour of the drawing towards the bottom of the gear in an effort to make less work for the tiny cutter your going to need to fit into the root areas of the teeth.
If you don't mind running the death out of your cnc mill, you can skip the part about manually making a blank. You can add a square or ring around your gear on each layer of your cad drawing to represent your piece of stock, then program each slice as a inside pocket operation.
Also, when designing my gear in Gearotic, I set shaft size to 0. That way after slicing it up, I don't have to worry about getting rid of the shaft holes in the cad drawing.
I grew a bunch of extra grey hairs trying figure out how to do this. Hopefully you guys won't!
Cheers,
Step 1 : Design your Bevel Gear in Gearotic. Its mostly about the tooth count and shaft angles at this point . Do yourself a favor and make the gear significantly wider than the finished gear you will be needing, as you will need the extra data further along for the machining process. As long as the tooth count and shaft angles are correct, the gear you need will be somewhere in there, within the extra long gear you just created.
Step 2 : Select your gear and go to the DFX output in Gearotic and spit out a 2D drawing of your gear. Use the side on view of this drawing as a guide to manually machine a gear blank out of whatever material it is that you desire to make your gear from. Make sure to center drill the gear blank or make your shaft bore. Just remember you will want some way of indicating where your center point is for setup later in the CNC. Also make sure you have a way of mounting this blank later on in your cnc mill. Usually the gear will need a shoulder on the backside anyway.
Step 3: In Gearotic, right click on your gear in the project tree and click "send selected to slicing module". Flip the gear using the perspective controls so you are looking at the gear from the back side. You do this as slicing starts from the bottom up, as would be needed for 3d printing. But we need the information in reverse, as cnc milling is generally done from top down. Next set your slice thickness. Keep in mind that the slice thickness you use now will also need to be your cutting depth for each pass on in your machining operation. Thinner slices will equal better resolution and less finish work on your gear later. But your CAD and program files will be much larger and your machining process will also be longer with very thin slices. My happy medium so far is .020 thickness. Go ahead and hit that slice button. Then you go down to the slice viewer slide bar, and have a look at how many slices you will need to form your gear. Make a note of what slice number that the outside contour starts to go back under the outside tip of the gear teeth. Any slice number past this will be no good as a milling tool cannot reach underneath the tip of the tooth and if these slices were programmed for milling, the machine would in turn mill off the majority of your outer tooth profile. Remember in step 1, when I said make your gear thicker than what you need? This is why. You need that thick gear design so you have a contour to follow all the way down to the root of the teeth. The last several passes of your machining operation your cutter will be "out in space" machining the tips of imaginary teeth as the real teeth ended long ago, but the cutter will be then coming back in and cutting metal out from the root area. Now you can select "0,0,0" option under "output slice" and click the "DFX Out" button.
Step 4: Go ahead and fire up SheetCam TNG! everybody's got sheetcam, right? Next Import your new sliced up gear drawing into Sheetcam. Make sure to select "Center Drawing on 0,0" when importing. This will automatically put the centre of your gear on x0,y0. Making everything way easier for setup and machining. Also For some reason, Gearotic puts loads of empty layers in its DFX output file. If you wanna be a rockstar, you can first use your favourite 2d CAD and delete all that extra crap before loading it into Sheetcam. You can also delete the slices that go back underneath the lower gear tip that I described in step 3. Now comes the really AWFUL NASTY TERRIBLE PART. You've gotta program a separate outside contour operation in Sheetcam for each slice, starting at slice 1 and going all the way down till the last slice before your contour starts to go underneath the outer tooth tips. ( if you didn't already delete them). IT IS SUPER IMPORTANT that you program each operation's depth of cut to the exact thickness that you made your slices in step 3. And that each successive slice's starting depth is exactly that of the previous slice's finish depth. If you don't do it right your gear will come out dis-proportioned or you'll break some stuff. Then go ahead and post your G-code with whatever post processor your mill unit can read.
Step 5: Mount your gear blank in your CNC mill. I clamp a 3 jaw to the mill table and grab onto the shoulder of the gear, of course with the bevel facing up toward the spindle. Zero everything up in the center of your blank, cross your fingers and hit the whatever it is you got for a go-go button. See what happens!
AFTERTHOUGHTS:
You may want to program a large endmill to make a few laps around the largest contour of the drawing towards the bottom of the gear in an effort to make less work for the tiny cutter your going to need to fit into the root areas of the teeth.
If you don't mind running the death out of your cnc mill, you can skip the part about manually making a blank. You can add a square or ring around your gear on each layer of your cad drawing to represent your piece of stock, then program each slice as a inside pocket operation.
Also, when designing my gear in Gearotic, I set shaft size to 0. That way after slicing it up, I don't have to worry about getting rid of the shaft holes in the cad drawing.
I grew a bunch of extra grey hairs trying figure out how to do this. Hopefully you guys won't!
Cheers,