The rpms were probably a little too fast. You want the surfacing bit to move somewhat slow across the wood so the rpms should also slow down or the bit is turning too fast in one spot.
1 Like
Burning means you are running too slow. Increase the IPM and possibly lower the depth of cut. The big 1" or larger surfacing bits create a lot of friction. Maple and cherry are the worst woods for burning. The cherry has a lot of resin inside and even cutting with a sharp table saw blade can produce burning. The key to eleminate burning on a table saw is to run the board through the blade fast. The same is true for the cnc. The big blade slows down at the corners to make the turn and you often get burning in the direction changes.
So increase IPM and decrease depth of cut. The router speed could be too high as @Brew indicated but 18K or so should work. If you still get burns try increasing the IPM 10-20% at a time.
4 Likes
Ok I will try the increased speeds and see if that makes a difference . Do you think if I take a shallow pass at faster speeds will it help correct my problem
I recently needed to resurface some face grain cherry and completely surface and un twist rough sawn hard maple. I found that setting a raster path that changed direction off of the work piece, a shallow depth of cut (0.01"), a very high feed rate 100-200 IPM (programmed 100 and used the override to keep bumping it up as long as it sounded and looked good), and cleaning the bit before each run to get the resin off the bit work well. I use a CMT citrus blade cleaner and a toothbrush. I was running 1800rpm but will slow it down the next time I need to deal with these issues. The cherry cut like butter and I could really fly with the light depth of cut but it deposited more resin on the bit. The maple kept me on my toes, and the reset override button, because the grain was challenging and had areas that were much harder, it also was not flat when I started so the load changed throughout the first few passes.
2 Likes
How do I set up a raster pass in carbide create. I do not see a setting for that function
1 Like
Carbide Create does not have that feature — you will need to draw the path you want by hand as a Curve or Polyline
See:
1 Like
Does carbide create pro have the raster feature?
1 Like
No, if this were a specific Pro feature I would have mentioned it.
I suppose you could model a flat surface and then use 3D Roughing and Finishing toolpaths to cut it — that should result in a raster pass, and the 3D Finishing toolpaths afford the option of angle.
By doing that, how does that translate into a tool path? Also, when designing this tool path,what size should the grid spacing be, half inch?
Model the area you wish to cut relative to the origin:
Then create an area larger by a bit less than the diameter of the tool which you will be using:
modeling it to be a bit less than Depth per Pass less than the Stock Thickness:
Assign a 3D finishing toolpath to that which will only cut to that thickness less than the depth per pass:
Note that you will get a raster path in whatever angle/direction you specify:
If drawing up manually, I would set the grid spacing to match the desired stepover.
1 Like
Odd thought. (I’m nowhere near the software to check this, so it could be a crappy suggestion). Can you fake out a raster using the engrave tool path?
(I’m trying to remember, is that pro only? A little challenge to keep capabilities of CC, CCPro, Vectric desktop and fusion 360 straight)
Just a random thought at breakfast.
John
Reply to my own reply
Made it to my computer with Carbide Create Pro and it looks like a Raster can be set up with the Engrave toolpath.
YMMV since I have not actually run this. (I thought of this since I remember the early version of engrave had an issue with setting rpm to zero)
John
Good point.
Yes, Engrave pretty much does a raster toolpath, but adds a pass around the perimeter.
Ok guys, correct me if I’m off base as I am new to all of this CNC and CAD design but I have been working on a design for a tool path here for the last hour. In carbide design, I made my work piece 1 inch larger in both directions than the actual piece . Then created half circles and poly lines across the entire work piece, with the half circles just off the edge top and bottom then connected the half circles with straight poly lines . Then when I went to tool path I use a contour path with a surface bit and it looks like in simulation, it going to do exactly what I need. Does this look right to you experienced makers???
This looks like the raster you referred to earlier
Yes, I would do that if I didn’t have Vectric V-carve where it is an option in pocketing. Circular returns make it fancy and smoother but as long as the bit is off the work you are good.
1 Like
That didn’t work so I tried a different approach and that worked . I did a poly line across the board an inch apart then created a tool path for each line separately. I had to design the set up to be larger than the actual work piece so the cutter would go completely off the work piece before moving over to cut the next tool path
Aside from feeds and speed, I have seen a tram issue (router/spindle not being square to the bed) cause something similar with larger bits (1”+).
Not sure if your passes are set along the y or x axis, try swapping them with you poly line to see if that helps. If so, may need to square the router.
If you are out of tram nothing helps but tramming. I agree that the bigger the bit the more it shows up if out of tram. Short of tramming decrease the step over. All CNC machines are not perfectly trammed so if a sanding pass over the surface makes it disappear that would work. End grain is much tougher to machine and sand than face grain.
If you think you need to tram a cheap set of 123 blocks will help. Jog your machine down close to a 123 block and power off machine. Then manually turn your Z down to touch the 123 block. Then if there is any space on one side use the eccentrics to adjust. Then turn the 123 block 90 degrees and test that the router mount is touching on front and back. For front to back you have to shim the Z assembly. You can use paper or aluminum foil folded up to get the front to back tram.
It is easier to remove the router and just deal with the router mount. You can leave the router in but it is very simple to remove it.
They also make some dual dial indicators that fit into the router collet. That is more complicated then the simple 123 blocks. After you get your router trammed then surface your spoilboard. A prerequisite is that your machine is square and level.
Rpms are too high.
I surfaced some cherry and oak recently.
60 in/min @ 11000 rpm. Seemed to help A LOT!
I did still get some discoloration but it was no longer burning.
Hope this helps
4 Likes
This topic was automatically closed after 30 days. New replies are no longer allowed.