Hi guys. I would like to carve this piece (The last supper):
Material: Oak
Width: 18.275"
Height: 13.748"
Thickness: 1.135"
I already did the roughing pass with a 1/4 upcut endmill
The problem is that in the finish pass the machine wants to do like a profile pass almost -0.5" depht in some parts before carving the center
Here is a video of this:
It does like 16 loops at 0.2", 0.3" - max depht like 0.45" in some parts
Do you guys think the 1/16 tapered ball nose can endure this? I let it run for a moment but I had to pause it since I was a little bit scared about the depht it was going (and of course the awful noises that it was making). What do you guys think? Thanks.
Edit: Those dephts are not recommended for the tapered ball noses. Iāll try to create a second roughing pass with a smaller bit like a 1/8 ballnose to see if I can cut wood in those smaller and depht parts of the piece.
Edit 2: My CNC master suggested to use a 1/4 ballnose for a first finish pass, that seems to be the best solution. Iāll update the post after I test this.
This is what Iām suposse to get after using the 1/4 ballnose for a first finish pass:
This eliminates most of the wood so the 1/16 tapered ballnose can do itās job without any danger I hope.
I would suggest preparing a simple test file in Carbide Create which makes the same sort of cuts as you are having difficulty w/ when using Vectric, make note of the current zero and try the test file out on the scrap.
See how the test works out and if it reveals a problem w/ the machine, let us know at support@carbide3d.com and weāll get it sorted out.
I believe Iām just worried to know if a 1/16 tapered ball nose can endure 0.5" depths of cut in some areas for the first loops, the machine is working perfectlyā¦ I just donāt want to destroy something by pure ignorance.
I donāt know how that works in Vectric (I found it really confusing and annoying to use) ā thatās not the case for Carbide Create, which is why I suggested testing w/ it.
Hi Will, I just realized I was wrong, like you suggested the bit really lost the Z and endep up cutting deeper that it should, it even completly lost the direction at the end. What can I do to avoid this next time?
This is really weird to me since I used the same zero (using the bitsetter) to use a 1/4 tapered ballnose to try to cut more wood of the project and it worked perfectly.
-Maybe the bit slipped but this doesnāt explain the lost of direction at the end
-Maybe the file was too big, itās 50MB
Reduce tool stick out by setting it deeper into the collet if possible.
Lower retract height, make sure to clear clamps and other hold down devices used.
As Will always says, add geometry to avoid slotting.
Now that I understand the problem I can remember that once I pressed ārun fileā and the bit position himself in the X-Y-Z, the Z did a weird sound (Like triying to go more up - the red light of the Z sensor was even on) I always though that this was normalā¦ Do I have to set up this for each work some way? I guess the easy fix here was to insert the bit deeper in the collet.
Sounds like your gcode is asking the z axis to climb beyond its upper limit and when it tries to, the a steps are getting lost (the grinding noise).
I carved a montage of Davidās hand touching God, framed in pillars and such like, to make a pair of very ornate cupboard doors - and Vectrics did a perfect job once I had sorted out max/min z-travel, and getting my head around overlapped ātilingā where the artwork exceeded the size of my machine in X.
Persevere, it is well worth it when you finally see the results
Could you please tell me what do you do to avoid climbing beyond itās upper limit? I guess I should had inserted the bit depper in the collet, but, is there another way? Or i just need to avoid the Z sensor red light before starting a job?
Itās a combination of tool stick-out, z range, where in the range you set zero, and the z range required for the carving. Itās not complex maths to figure out a āgoodā setup for your job, but it does take a few goes (and even a few mistakes) to understand what is happening.
One observation from your pictures is the huge stick out of the tapered BN cutter - that eats up your usable z rangeā¦ I would see if it is possible to inset the cutter into the collet up to say 5-10mm above the colour change mark where the flutes stop
Most likely the odd noise indicates that steps were lost on retract due to a wiring issue ā let us know about this at support@carbide3d.com and weāll get it sorted out.
If you can upload the Vectrics file, either on This forum or if too big, put a link here to where you can upload (OneDrive, GoogleDrive etc), and I will take a look and see if a few pointers will help. It would be useful to know your machine size in XYZ and type of z axis to do this
Another observation is that the 1/4" end mill cannot get into the fine detail of this carving, but the 0.0313" TBN cutter can, and the GCODE output from Vectric is trying to do just that. I would step down 1/4" to 1/8" to 1/16" and finally your TBN - VCarve will let you choose multiple tools (called REST machining) to take out the bulk of material with the 1/4", move into the finer areas and remove the next level of bulk with the 1/8" etc. Finally the TBN can get in and produce the super-fine end result.
So I think you have several issues going on at the same time:
Running out of Z-axis travel, most likely the major factor here is the amount of tool stick-out (it looks like 3" or more in addition to the depth of your carving (1.135") and a safety clearance (typically 0.5"). All these together is 4.635" and may exceed the possible travel.
The 1/4" cutter canāt get very far into the fine detail, which itself is quite deep. When switching to the 0.031" TBN cutter it tries to remove this depth around the fine details - but the stress on the tool is risky, and the additional risk of the machine losing XY steps and thus losing position owing to the excessive cutting forces. This will be true whether using Vectrics VCarve, CC or Fusion as the software algorithms to do this tend to be broadly the same. Step down tool size in āhalf sizesā is a reasonable rule here - 1/4 to 1/8 to 1/16 to 1/32 (or TBN) and that way the smaller cutters get less stress.
I downloaded your RAR file and noticed that some of the detail of the model contains vertical walls that the TBN will have to follow - the taper means that higher up the wall the shank of the TBN will touch/cut and a) spoil or somewhat spoil your carving, b) increased cutter forces as this āshank cutā was not expected (or the software algorithm is too stupid to notice the risk)
Personally, I wouldnāt output the whole lot as a single file and let BitSetter (whatever the tool change checker is called) sort out the tool length differences. Output the files for each tool separately and run each one as its own ājobā on the machine - that way if there is an issue you can start that job again (painful in terms of time, but not as painful as having to run the whole thing from the start again). There is nothing wrong with the BitSetter device, and many people swear by them, but the time saving promise from my thinking is marginal at best - the only time I can think of a big advantage is if you have machined away your z-zero reference material and you need the machine to ārememberā where that was to setup the next cutter
