Cutting Observations of a Newbie

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro
KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Cutting Observations of a Newbie

Post by KevinC »

So I've been at this for a little while now. Long enough to build my machine and learn how to maneuver it, create Vectric Files and toolpaths and make cuts on my machine.

This weekend I was attempting my first project to cut some round catch-all trays with some v-carve engraving in the bottom of them. I was using a 90° v-bit at a 0.1" doc and my results were rather disappointing. They are not clean and there is wood fur like material in a lot of the grooves. Is this common? Also, the cuts were bleeding over into other cuts making the edges uneven and blotchy. The trays are a 6" circle and I attempted to chamfer the top inside and outside edges with a 90° v-bit. But when I cut the inside with a bowl bit and the outside with an endmill the cuts did not meet up with the bottom edge of the chamfer. Cutting to just the outside of the lines I had chosen for the toolpaths. This left a small groove where the point of the v-bit was. Next the v-bit engraved a shape where I then used a 1/8” End Mill for Clearing the material. But the endmill did not go to the bottom of where the point of the v-bit did, leaving a raised middle with a small groove around the outer edge.

In my V-Carve Pro the image of the simulated job looks clean and crisp. So, is this a machine thing? Do I still have fine tuning that is needing to be done? Or is this like a step over thing or something software related? Is it a depth of cut thing? Or do I just need to accept my results and try to work with them? What if I used a 60° bit? Would that give me better detail on my v-carve?

Any direction would be greatly appreciated.

Kevin

pixl8ed
Posts: 11
Joined: Sat Sep 26, 2015 9:54 pm
Model of CNC Machine: CNCRP Pro4896, Laguna Smartshop 1
Location: SoCal

Re: Cutting Observations of a Newbie

Post by pixl8ed »

This sounds like an issue with zeroing the different bits. If you're setting the Z manually, you might be zeroing the vbit a touch low.
Also, try to zero the bits in the same XY spot on the material or spoilboard -- if the material or spoilboard isn't perfectly flat, zeroing in different XY locations can give different results :oops:

KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Re: Cutting Observations of a Newbie

Post by KevinC »

Ya know that's a good point pixl8ed. I did have to re-zero a couple of times because after my first zero too much of my v-bit shaft was exposed for me to feel comfortable cutting with it so I lowered it. Then when it came time to cut my profile on the outside I had to raise my zed. I used the touch probe at first but then the paper technique after and then back to the touch probe. But thinking about it the engraving and the clearing cuts were done on the same z setting so that doesn't explain why my clearing cut didn't cut all the way to the bottom.

I plan on trying these again but this time making sure my bit changes can happen without having to change any of my work area homes. I am curious to see if that will make a difference.

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Cutting Observations of a Newbie

Post by martin54 »

Kind of a difficult question to answer as there isn't really enough detail & there are so many thinks that could have caused some of your issues. The actual CRV file you are using (copyright permitting) &/or screenshots plus pictures of the actual machined results can help a lot & you will generally get better replies when people can see what is going on rather than try & guess :lol: :lol: :lol:

What material were you machining? Wood of some sort I know but there are lots of different types & you can't machine them all exactly the same way :lol:

The toolpath preview is very accurate so if your machining results were not the same then it's more than likely the problem lies somewhere outside of the software, either with the post processor used, the CNC control software, the actual machine or the way the job was set up.

I plan on trying these again but this time making sure my bit changes can happen without having to change any of my work area homes. I am curious to see if that will make a difference.
I don't understand this bit, Once you have your material placed on the spoilboard & have set your X Y Z zero positions for the job then you should never alter the X & Y zero positions. You do however have to re zero your z axis everytime you do a bit change, As has been said already if you are setting your z zero to the material surface try to use exactly the same spot when you re zero the z axis just incase the material surface is not completely flat. I generally put a small pencil X on the work piece for reference rather than try & remember :lol:

User avatar
gkas
Vectric Wizard
Posts: 1450
Joined: Sun Jan 01, 2017 3:39 am
Model of CNC Machine: Aspire, Axiom AR8 Pro+, Axiom 4.2W Laser
Location: Southern California

Re: Cutting Observations of a Newbie

Post by gkas »

Another comment... Carving with a Vbit @ 0.1" depth needs a very accurate surface. The wood MUST BE FLAT. If you don't have a drum sander, etc, then plane off a tad from the surface with a flat bit. This will guarantee a flat surface for the Vbit. Use a pencil to scribble over the entire surface. All marks will be gone when the surface is planed flat.

KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Re: Cutting Observations of a Newbie

Post by KevinC »

Yeah I was afraid of that Martin. I can post the CRV file and the screen shot of the toolpath preview now and then get some pictures of the final pieces when I get home tonight. Probably post them tomorrow first thing.

The material I'm machining is oak and walnut.

I'm running a Workbee CNC with a Duet Control Board. The name of the Post Processor is Duet Arcs (mm). I can't find the file for you to view but it is in the V-Carve List of Post Processor to choose from.

Let me try to explain the comment I made that you didn't understand.

So I have a fairly large bed. I placed 6 - 6"X6" blocks on the bed and anchored them with double sided tape. My machine has its machine home and it's work area home. I am able to save 9 work areas each with their own zero X,Y,Z. I have an X,Y and Z probe that will locate all three positions for me and I save each one to its own work area. I used a 1/4" end mill to do this and then switched to my bowl bit. It cut fine. But then I changed to my V-Bit and discovered I had way more shaft of the end mill exposed than the v-bit has available when I zeroed everything out. So I had to move my z down so more of the shaft of the V-Bit was in the router. I went to the top corner of each workpiece and zeroed my Z to the V-Bit. Made my cuts. Changed to an 1/8" End Mill to Clear what the V-Bit couldn't by placing the end mill loosely in the chuck and the homing the work area. It would push the bit into the chuck as it went to z zero. Once that was done I had to change my Z back to accommodate my 1/4" End Mill to make my profile cuts for each piece. To do this I used my X,Y and Z probe again and zeroed everything out and cut my pieces out. Once Pixel8ed pointed out that this could cause a problem the light bulb went off. I'm sure a lot of my issues are because of how I handled my work area zero's. So when I do my next round of these trays I'm going to zero each of them out in a manner that will provide enough depth to hold more of the v-bit shaft in the chuck and enough clearance that the 1/4" End Mill can make it's final profile cut.

I'm sure that's clear as mud. LOL...

I do have some pictures I was taking as I was going through the process I just don't have any of the final product. So I'll post what I have next and then get some pix of the final cuts and better examples of what happened tonight and post them tomorrow.

Kevin.

KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Re: Cutting Observations of a Newbie

Post by KevinC »

gkas wrote:
Tue Sep 21, 2021 3:54 am
Another comment... Carving with a Vbit @ 0.1" depth needs a very accurate surface. The wood MUST BE FLAT. If you don't have a drum sander, etc, then plane off a tad from the surface with a flat bit. This will guarantee a flat surface for the Vbit. Use a pencil to scribble over the entire surface. All marks will be gone when the surface is planed flat.
Already learned that mistake the hard way Gkas. LOL.... this time I ran everything through my plainer until all of them were the same thickness. 0.7"... I should also add that I have milled my spoiler board down so it's perpendicular to my X axis as well.

KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Re: Cutting Observations of a Newbie

Post by KevinC »

Here's the goal...
Collins Catch-All Tray.png
Here's the CRV File
Collins Catch-All Tray.crv
(1.18 MiB) Downloaded 89 times


6 Work Areas
IMG_3562.png
First cut
IMG_3564.png
Bowl Cut
IMG_3565.png
IMG_3566.png
IMG_3567.png
Have at it guys.

User avatar
Tex_Lawrence
Vectric Wizard
Posts: 932
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko3XXL; JTech7W; V-CarvePro 11.554
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: Cutting Observations of a Newbie

Post by Tex_Lawrence »

KevinC wrote:
Tue Sep 21, 2021 8:55 pm
Here's the goal...
... Have at it guys.
Kevin, you're making this too hard on yourself, especially for your first project.

Just do one of them at a time. Get a corner fixture reference, so you can place them in it one after another and keep the same CNC settings for each one. That way you use one toolpath for one part.

Get your XY zero correct. In the photos it looks like your Y zero is not set correctly. Your walnut-looking stripe will not be centered.

The photos look like you used the ballnose bit for clearing out the whole pocket, so it left a groove in the bottom. You must have a large stepover setting. Perhaps use an end mill for clearance of a pocket up to the point where the ballnose can finish with that rounded inside corner.

PS. If I were to do multiples like this, I would place them all together edge-to-edge and use "Plate production". YMMV.
Tex — Crooked Wood Products
Now there's a man with an open mind – you can feel the breeze from here.

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Cutting Observations of a Newbie

Post by martin54 »

OK firstly my understanding of machine/stock positions is a little different to Vectrics, I started with mach3 so you would need to watch their tutorials on coordinate systems to understand but I won't go into it as that may confuse people, especially those who don't have homing switches :lol: :lol: :lol:
So my understanding of what you are doing is you are homing your machine by sending it a a particular position that references the spindle/router to your machine table. You are then setting up a number of work offsets where your stock material is placed, probably using G54 - G59 moves for this but not being an expert on different CNC control systems that is just an assumption.
You use your corner finder to set up each of these positions on the spoilboard.
My guess would be so you can machine all 6 with each bit before before doing a bit change.

But then I changed to my V-Bit and discovered I had way more shaft of the end mill exposed than the v-bit has available when I zeroed everything out.

this was the bit that I didn't really unserstand, until you added this bit :lol: :lol:

Changed to an 1/8" End Mill to Clear what the V-Bit couldn't by placing the end mill loosely in the chuck and the homing the work area

Now this is only my own expereince but I did try this at one time & then dismissed the idea because I don't think you can set it accurately enough, I found that no matter how I tried the bit would move within the collet when I was trying to tighten it & I didn't get the accuracy I was looking for, this may well be why your V bit & endmill machining have different depths.

When I do a bit change I just stick the required bit in the chuck & then reset my z zero position, quck & easy to do once you have done it a few times. :lol: :lol:
Doing it that way would however require you alter your z zero position for each of your work pieces.

So whats your process from start to finish? I don't do production type work but if I were doing what you are with the size of your machine then I might approach it slightly differently. I would probably experiment but my first plan would be to prep & glue up one length of Oak/walnut board. Once that was done I would leave it as one length, place that on the machine & then do the rest of the process on the CNC machine :lol:
Saves time cutting the board into lengths & time setting up the individual work offsets, still gives you very few bit changes.
If you can't do that & have to have seperate pieces then I would probably do what Tex_Lawrence has suggested & set up a jig/work fixture & do them one at a time, each operation could be carried out before moving on to the next bit that way but it would require more time stood at the machine

Tex_Lawrence Not looked at the file but in the original post be said he was using a bowl bit rather than a ballnose bit, reducing the stepover however will give better results even with a bowl bit :lol: :lol:

KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Re: Cutting Observations of a Newbie

Post by KevinC »

Martin that is a brilliant idea for mass producing these things. If I was to sell these I would need a way to do it as efficiently as possible. One piece cut in half, one glue up with a strip of walnut in the middle and one mount up to the spoil board would save a ton of time. But you are saying to re-zero my Z after every tool change with my probe rather than using the loose bit in the collet technique? It makes since. The probe should or would be way more accurate than the other method. If my machine is dialed in. I never thought of letting the machine do all the cutting but it already is. I was cutting 6" blocks, ripping them in half and then gluing them all up. Man there is really some outside of the box way of thinking with CNC stuff. I get so wrapped up in the individual method of approaching things. It never dawned on me to let the machine do all the cutting. Good grief. I feel a little stupid at the moment. HOWEVER... I am still learning so this time I get a pass. LOL...

Next I need thoughts on the tear out and roughness of my v-carve cuts. See image below.

Here's the final look of one of them.
IMG_3585.JPG
Notice the tear out and rough edges? Should it be that way? Or is my bit dull. Or my feed rate to slow or my router speed too slow or the wrong bit all together? Should I use a 60 degree bit instead? I need the v-carve to be as smooth as possible so I don't have a lot of clean up in the end.

I have more images if you want more just say so.

KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Re: Cutting Observations of a Newbie

Post by KevinC »

Tex I could definitely place a 90° jig on there and just cut from the same place every time. In fact I plan to do that on some other projects. I thought by having all 6 locations zeroed in, it would speed up the process and make things simpler. But I see now how I'm working harder and not smarter. This thread is teaching me a great deal on production. I spent all this time learning how to build the machine, then learning how to make it move, then running test cuts to determine proper feeds and speeds. Now it's learning how to cut stuff. Thanks for the Jig idea Tex. I will do that.

KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Re: Cutting Observations of a Newbie

Post by KevinC »

I should also mention my feed rate was too fast for my router at 160 IPM and a Plunge Rate of 20 IPM at 18,000 RPM.

So I changed it to a feed rate of 65 IPM and a plunge rate of 32 IPM at a router speed of 18,000 RPM.

Is that too slow?

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Cutting Observations of a Newbie

Post by martin54 »

There are quite a lot of posts on vcarving & tearout so a search on the forum might help & throw up a lot of good info. If it is detailed work then slowing your speed & feed rates can help, you may also need to reduce your depth of cut, using a sanding sealer prior to cutting sometimes helps as it helps to bind the fibres together, if its a deep carve then you may need to apply more than once as you progress to ensure it has soaked in deep enough. Use a fast drying sealer & you can also thin it down to help it soak in deeper.
Sharp bits are a must for this & also running the toolpath a second time can help with clean up & leave less hand finishing.
What spepover are you using for your bowl bit for the pocket? Even with a flat bottom cutting bit you get a better finish with a smaller stepover but that will add extra time to the toolpath for each pocket. To overcome this I quite often set up 2 seperate toolpaths for a pocket cut, first one with the normal start depth & a cut depth just short of my finish depth using the normal stepover. The second toolpath I use the depth that my first toolpath cut to as my start depth & then cut to my final depth using somewhere between 15 - 25 % stepover. Output the 2 as one file so they cut together. It means the machine roughs out most of the material at the normal speed but then the last pass is with the smaller stepover for a nice finish at the bottom of the pocket.

I'm not saying your loose bit in the collet won't work, I am just saying that I could never get it to work accurately enough myself so don't use it :lol: :lol:

I spent 20 years in the Royal Navy as an engineer & a lot of the job was problem solving so if I have any sort of work to do I think it through & then try to plan the best & most efficent way to complete it so it's not just down to CNC work for me. My CNC machine is just another tool in my workshop, it can be very easy to use the CNC for jobs that would be better done or quicker using another piece of equipment such as a table saw or router table so you need to watch out for that but in this case it makes sense to me to cut them mostly on the CNC machine. Others may disagree & have a better more efficient way. As I said before I don't do production work myself & I am not set up to do it.

KevinC
Vectric Apprentice
Posts: 57
Joined: Fri Dec 11, 2020 10:31 pm
Model of CNC Machine: WorkBee CNC
Location: Minnesota

Re: Cutting Observations of a Newbie

Post by KevinC »

Okay new project similar issues. This time the material is MDF and there was NO load on the router when it cut.

Here's the file
Home is where you duke the hardest.crv
(2.08 MiB) Downloaded 54 times
Here's the results
IMG_3797.JPG
IMG_3798.JPG
IMG_3799.JPG
IMG_3800.JPG
IMG_3801.JPG
I used my touch plate between bit changes too. So the depth should be spot on. My spoiler board looks like this.
IMG_3803.JPG
The lines you see are just that. Lines. If you run your fingers over it you can't feel any ridges so the spoiler board is parallel to the X axis.

Thoughts Gentlemen?

Post Reply