Surface finish issues in 3D carves

AaronMatthews · February 26, 2016, 6:41pm

Continuing the discussion from 3D Dragon carve in red oak:
Any thoughts or input would be appreciated.

I have been having some issues with “ripples” in the surface of 3D carves.
Other people have mentioned having them when they cut too fast. So ultimately slowing down will probably be the fix for the issue but I want to try to figure out what exactly is going on to see if it is a symptom of an issue I can fix.

So I have started to run some carve tests to see what settings and strategies will have an effect.

Both parts were carved at the same time from the same piece of wood using the same bits.
(I did not carve out the mouth and eyes on one and used different stains on each to help tell them apart later)

Software: Vcarve pro and UGS
Model: VCarve clipart purchased from Design and Make (designed for a 1/8" ball nose bit)
Material: Cedar Fence Plank (well seasoned)

Carve #1 (on the left of the first picture) is the control, using the same settings that have been giving me issues. Feeds and speeds were calculated with GWizard.

Bit: 3.175mm Ball Nose [1/8 inch]
Width of Cut: .0318mm (10%) [0.0125 inch]
Feed: 3314.6 mm/min [130.5 inch/min]
Speed: 27000 (#6) rpm
Strategy: Offset (spiral), Climb
Depth of Cut: 0.66mm (machining allowance from rough cut) [0.026 inch]
Finished with Minwax “Gunstock” stain and Tongue Oil

Carve #2 (on the right of the first picture) is the first test, using modified settings. Feeds and speeds were calculated with GWizard.

Bit: 3.175mm Ball Nose [1/8 inch]
Width of Cut: 0.318mm (10%) [0.0125 inch]
Feed: 3314.6 mm/min [130.5 inch/min]
Speed: 27000 (#6) rpm
Strategy: Raster (up and down), 90 deg (Y axis)
Depth of Cut: 0.66mm (machining allowance from rough cut) [0.026 inch]
Finished with Minwax Pastel “Cranberry” stain and Tongue Oil

Close-up of the first carve:

If you look carefully you can see the “vein like” ripples in the surface. These follow the couture of the cut path at a 90 deg angle. This same pattern has been showing up even when I scale the model larger or smaller and run it at different feeds. It is not in the model or G-Code (I have triple checked)

Close-up of the second carve:

The “vein like” ripples are completely gone!
There are very noticeable groves running along the cut lines up and down the carve.
It is very hard for me to tell by eye but it looks like every other cut line is just a bit deeper. I will have to get my calipers out and measure to be sure

The “groves” are much more noticeable on the knot hole next to the nose.

So this lead me to theorize that the bit is deflecting more when moving down on the Y axis as opposed to moving up. This is harder to visualize on the offset (spiral) carve because it is a curve following the couture of the model. But when it first starts out it is basically a up and down carve.
So I took a closer look at the start point of the first carve which is the nose.

It is a little hard to see in this photo but on the right side of the nose, where the bit moves down along the Y axis, there is a prominent ripple. While the left side of the nose, where the bit moves up along the Y axis it is smooth.
This is not present in the raster carve

(I had noticed this effect on another carve but had mistakenly assumed it was due to a change in hardness in the grain of the wood)

So I am thinking this a deflection / chatter issue.

I know from earlier tests with 2D carving that my XC is very prone to chatter when climb carving along the X axis. (which is why when I Raster carve I always do the main movement along the y axis) And that a reduced feed rate lessons the chatter but does not eliminate it. Switching to a Conventional strategy does.

So I think the next test will be to do the same carves but Conventional rather than Climb and Raster along the X axis instead of the Y axis and see what happens.

Earwigger · February 26, 2016, 9:58pm

I look forward to seeing the result.

Aside from the typical scalloping, these are not bad for moving that fast. I typically 3d carve at 40 inches per minute with an 1/8" ballnose after a roughing pass. Sometimes, that little bit has to remove a LOT of material, and you may be correct with it appearing to struggle more one way rather than the other. It seems to me you are cutting very, very fast. Of course, I have only 3D carved in very hard woods. If it helps, this walnut 3d carve was a 1/8" ball nose, 25 inches per minute and 10% stepover. I still see plenty of scalloping here and results are not any better than you achieved. I hope with the input of others we can figure out some improvements.

AaronMatthews · February 26, 2016, 10:36pm

The feed numbers GWizard are giving me are very fast. Part of the problem is that these numbers are based on the optimal speeds that the bit can take, not the machine.
There are settings for how much “flex” your machine has but I have no idea how to measure it for the XC.
From what I can tell the rails on the XC will start to flex long before the bit will (at least with a larger bit)
I realize that the math for the amount of twist being put on the gantry is completely different from the amount of flex in the bit but I am hoping it is close enough that I can use it to make the generalization that “these settings cause more/less deflection than those”.

I would just chuck the number and start over except for 3 directions of travel (left, right and up) it is cutting nicely. Having a issue when it is moving in just one direction makes it seems like an alignment / v wheel problem?
I am using the steel bar stiffing mod which may be causing some spacing issues with my v wheels as well.
There is a lot to look at now that I have some idea where to start.

Ultimately, I think I will have to use slower feeds but I am hoping it is a minor speed reduction and not a whole order of magnitude.

AaronMatthews · February 26, 2016, 11:02pm

Love the carve! I have been playing around with soft woods because I don’t want to waste the good stuff on tests and learning projects.
But the hardwoods look and feel sooooo much nicer!
I was looking at first small oak box I made and even with it’s flaws I really like the way the oak looks and feels.

…

It is hard for me to see in your pic, but it looks like you have a “pencil line” just inside the inner edge? Where VCarve makes the first cut of the finishing pass? Is that what you mean by scalloping?

I am having a similar issue but I managed to figure out what was causing it and a workaround for it.

When VCarve does its 3D finishing cut on a complex shape it starts the first cut just inside the outer edge. The problem is this cut is at full bit thickness. Then after it makes that initial cut it can take the rest of the cuts at the normal step over.
Because this first cut is so aggressive it is causing the depth to be a bit off. (flex and deflection?)
Worse it cuts the “channel” then cuts the inside are, then the outside area so you can get this weird seam where they all line up. (Which I call a “pencil line”)

I suspect that if we had the option to enable Ramping on the 3D finishing carve this would not be an issue. (I wonder if I contact Ventric if they would add that as an option sometime?) So I did some testing and it turns out that if you “simplify” the object (no holes), VCarve with start with a single plunge cut in the center of the carve and spiral out from there. No more “seams”.

I used some of the 3D Tab clip art, scaled down very thin to “plug” the holes in the eyes and the mouth so the object was “sold” as far as the 3d carve was concerned. This changed the carve pattern and got rid of my “pencil line” seams.
I even modified the profile cuts so I can choose to cut out the mouth and eyes or leave them closed.

…
(Now that I think about it if I made the whole tiki sitting on a oval that would change the tool path of the 3d carve as well, which would impact the “ripple” issue as well.
I would have to run the numbers. Carving all that extra area might be no more of a time savings than just slowing down my feed rate. But it is a good trick to remember. It might come in handy for other projects.)

Earwigger · February 27, 2016, 12:19am

Dude - I have no idea. These scallops are easy to clean up, but if you can find a solution, I am all ears. I am certain that if this was my full time job, I would have developed a protocol by now.

ShaneBell · February 27, 2016, 3:07am

If you have a camcorder that allows time lapse video set it up to have x,y, and z axis in view. Replay video and you will see where your machine flexes at. i found this very helpful when doing stiffening mods. people seem to say alot about the x axis but i found that the y axis has far more movement than most might think. In the end the y axis mods helped reduce chatter and other artefacts in the 3d carvings more than the x axis mods.

AaronMatthews · February 27, 2016, 6:58pm

More testing.
First I checked over my XC.
I used an old tooth brush to clean out the dust in the v wheels and rails. (It worked really go and is now part of the tool kit)
Double checked that the v wheels were nor slipping or loose.
Took a hard look at the v wheels on the x gantry to make sure they were seated correctly and not pushed out of position by the steal bar stiffening mod. The looked fine.
Double checked that the pulleys were tight (I had a scare where I though the set screws were gone but they were there, just harder to see than I expected.

I then grabbed the spindle and started to push and pull, looking for any “wiggle” in anything and trying to figure out just what is flexing.

I discovered that the holding current on my Y motors was a bit low (if I pulled hard it would slip.) so I bumped that up a little bit.

The biggest “flex” was they Y axis moving just so slightly. I double checked everything and it looks like the movement is due to the belt stretching. So I tightened up the belts. That helped but did not eliminate it.
I kept pulling and pushing and it looks like the remain flex is the gantry rail twisting. It isn’t much, but even with the stiffening mod there is still a tiny bit of twist.
(I think this is approaching the limit of the materials. I don’t think I can do much to stiffen it up any more without changing the design. Going with a wider rail maybe?)

With that done I did another test.
As before 2 carves with the same piece of wood using the same bits. Just some minor modifications to the print strategies.

Carve #3
Feeds and speeds were calculated with GWizard.

Bit: 3.175mm Ball Nose [1/8 inch]
Width of Cut: .0318mm (10%) [0.0125 inch]
Feed: 3314.6 mm/min [130.5 inch/min]
Speed: 27000 (#6) rpm
Strategy: Raster (up and down), 0 deg (X axis)
Depth of Cut: 0.66mm (machining allowance from rough cut) [0.026 inch]
Finished with Minwax “Gunstock” stain and Tongue Oil

A much smoother carve. No more “every other line” being a different depth.
There are occasional lines that are off. I noticed that I had the RPM setting wrong for this carve. I fixed it and the reaming carve was smooth (above the eyebrow). I am not sure if the corrected RPM made the difference or not.

But this does show that the issue is in the Y axis movement.

Carve #4
Feeds and speeds were calculated with GWizard.

Bit: 3.175mm Ball Nose [1/8 inch]
Width of Cut: .0318mm (10%) [0.0125 inch]
Feed: 3314.6 mm/min [130.5 inch/min]
Speed: 27000 (#6) rpm
Strategy: Offset (spiral), Conventional
Depth of Cut: 0.66mm (machining allowance from rough cut) [0.026 inch]
Finished with Minwax “Gunstock” stain and Tongue Oil

I was hoping that this would fix the issue. It did not. It did lesson it a bit but it is still present in most of the carve.

There is still some ripple in the nose but now it is on both side equally.

I am thinking that some of the ripple is chatter from the climb strategy as certain ripples are gone competently. The rest are just from cutting to aggressively.

So I will start dialing back my settings, say 10% at a time, until the carve clears up.

I will be keeping a close watch on the carves to see if I can actually see it flexing.
I may even run some faster carves so it will be more prominent. Just to confirm my theory.

It has been a lot of work to get back the the initial solution of “slow down” but at least I know that is the fix as oppose to something like a loose v wheel.

Hopefully, I can use the new setting to figure out what the deflection threshold is for a clean carve so I can keep using GWizard to get optimized depth feeds and speeds.

ErikJenkins · February 27, 2016, 7:21pm

Try cutting with the grain, I get much better results when my passes are with the grain.

AaronMatthews · February 27, 2016, 8:05pm

Here is a rough example of what I am talking about.
Skull and Bones no Scallops.rar (9.3 MB)
(if you use this be sure to change it to your material thickness, bits and feed settings!)

Unfortunately, I had to extend the 3D backing to cover the whole model so this will be a long carve. But the VCarve will carve this as a single spiral, so no scallops where the multiple carves meet.

AaronMatthews · February 27, 2016, 8:09pm

Test number 2 was with the grain of the wood.
In my case I running the machine so fast that the variations in the grain density are to subtle to be an issue.
I think as I dial back the feeds and speeds it wit start to be noticeable. And once I hit that point I will know I am close

AaronMatthews · March 1, 2016, 2:47am

In setting up for the next set of surface tests I was going over older carves.
Many of which I was cutting deeper and faster with little to no texture issues.
Most of those just had bad pencil lines / scalloping which I did not realize was a separate tool path issue at the time.

Also I am going over my Feed and Speed calculations in G Wizard and getting very different results, even faster cut speeds, that before.

Something is very off with my calculations but on the side of conservative cutting.
I am going ahead and running 2 tests, 90% feed settings and an even more conservative defection setting in GW.

But I thinking, the numbers GW as been giving me have worked pretty well with my endmills. It is hard to tell with rough cuts but they gook pretty good. It just seems to be the ball nose.
I am beginning to think it may be just a dulling bit?
Or maybe I am cutting too conservatively and running into rubbing issues?

I recently got up a set of extra long bits for carving on a 2x12. (Mainly to make sure I have clearance for the final profile cuts)
I think I will go back to square one with the brand new bits and a fresh numbers and see what kind of results I get.

AaronMatthews · March 1, 2016, 4:45am

Found it! I had my ball nose entered as a 90deg angle (default) instead of a 30deg angle tip.
This will make a huge difference.

I also found some updated info on the machine settings. Borrowing some data from the Shapeoko 3 profile.
Not that it seems to be having much impact

AaronMatthews · March 1, 2016, 9:25pm

With that done I did another test.
As before 2 carves with the same piece of wood (some well seasoned cedar planks) using the same bits. Just some minor modifications to the print strategies.

Carve #5
Feeds and speeds were calculated with GWizard.
(Note I have sense found a error in my settings for these calculations)

Bit: 3.175mm Ball Nose [1/8 inch]
Width of Cut: .0318mm (10%) [0.0125 inch]
Feed: 2983.14 mm/min [117.4 inch/min] (a 10% reduction)
Speed: 27000 (#6) rpm
Strategy: Offset (spiral), Climb
Depth of Cut: 0.66mm (machining allowance from rough cut) [0.026 inch]
Finished with Minwax “Dark Walnut” stain and Tongue Oil

Not much change in the surface rippling. I think a more dramatic reduction in feed will be necessary to see a change.

Carve #6
Feeds and speeds were calculated with GWizard.
(Note I have sense found a error in my settings for these calculations)

Bit: 3.175mm Ball Nose [1/8 inch]
Width of Cut: .0318mm (10%) [0.0125 inch]
Feed: 1955.7 mm/min [76.9 inch/min]
Speed: 27000 (#6) rpm
Strategy: Raster (up and down), 0 deg (X axis)
Depth of Cut: 0.66mm (machining allowance from rough cut) [0.026 inch]
Finished with Minwax “Light Walnut” stain and Tongue Oil

I was supposed to do this one in a spiral cut strategy, but I forgot to make the change to the cut file.
But I am impressed with how much cleaner this carve came out.

Funny, 80 ipm just what everyone else has been doing
I expected this would be the case but it has been a good learning experience for me.

What I have learned so far

I found the settings error that was causing my ball nose numbers to be so wonky as compared to my end mill numbers. I am still getting very high feed rates, but the relationship between feed, rpm and depth of cut is different enough to have a effect.
I discovered that GWizard has the option to deflection optimize the feed rate for a specific width of cut and depth of cut. Using this mode I am getting numbers on par with what everyone else is using (80 ipm etc)
VCarve works under the assumption that you are using the same bit for roughing and finishing operations. This made me reconsider my strategies. What if I did 3 cuts instead of 2? A rough cut with a big bit, a rough cut with the finish bit, then the final cut. I was avoiding the really thin depts. of cuts GW was telling me I should use with the high feed rates because I don’t trust that I can reset the Z height that accurately when changing bits. (we are talking 0.2 mm or less). But if I don’t swap the bit this is no longer a problem. It is just a mater of seeing if I can reduce the cut time enough to be worth it.
*I really watched my machine carve. And to my eye I didn’t see anything flexing or twisting. But if it is bit deflection we are talking about values < 0.05 mm. Possibly even less if is the gantry twisting. However, I did notice that my XC shimmies and shudders a lot. I think I need to read up on acceleration and see what, if any, impact that could be having on this process.

ErikJenkins · March 1, 2016, 9:38pm

Nice bit of trial and error…so how many masks do you have now?

AaronMatthews · March 1, 2016, 9:43pm

About 14
Part of the reason for this post is for me to document my settings because I am looking at my earlier ones and can’t remember what settings I used. And of course I lost my hand written notes.

MartinLombana · March 1, 2016, 11:34pm

Nice Masks :D.

I am curious as how much time did it take you for all the passes to complete the carving.

Earwigger · March 2, 2016, 1:15am

You might find it helpful to change your settings in a meaningful way for each test before our planet is entirely deforested. Also - maybe try the settings that were presented to you when the thread began. Also, V-carve does not assume you are using the same bit. You can select the bit for each pass.

I know what YOUR family is getting for Christmas this year.

AaronMatthews · March 2, 2016, 5:45am

For both rough and finish, about 40 min on the earlier carves about 1 hour and 40 min for the slowest one.

AaronMatthews · March 3, 2016, 6:55pm

That was the plan for the latest batch but I screwed up and ran the wrong file and then had the spindle brushed die mid cut But it is on the schedule once I get up and running again.

The thing that started me down this path is that the first tiki I carved came out wonderful. (Just a bit of “Scalloping” which I know now how to correct for)
Then they started to come out with this weird surface finish using the same g code. I stared trying to figure out why, what changed?
I was at a loss. Because my numbers were kind of random I gave GWizard a try, figuring it might be my settings? And well, things kind of snowballed form there.
By they way, in writing this I realized one thing that changed just before I started having issues, I added my current dust shoe. The shoe is kind of improvised and I did not try to minimize weight and hose drag when I made it. Time to re-do it right!

LOL - I have been hording wood for “projects” for years. No able to bring myself to throw away “useful” wood. So I have this huge pile of partial planks and such.
I am almost giddy to finally be using it up.

That was supposed to be carve #6, but I screwed up and used the wrong the cut settings. I was re-doing it properly when my spindle died.

Let me clarify my statement on that. This is not a critique of the VCarve process. This is a commentary on my ignorance on how to use it properly.
Yes, you can select any bit you want for each operation using larger bits to clear away material significantly faster, as is the standard practice.
However, I noticed something setting up my project in VCarve.
First, when setting your machine allowance you get the error message:
“The allowance left is greater that 20% of the tool diameter. Leaving large allowances slows down the toolpath calculation time and may lead to finishing tool breakages.”
Second, you can not specify the Pass Depth on the finish machining toolpath. This is a problem because there a areas that the large bit I used can not carve out. Some of which will be so thick as to put a detrimental load on my finish bit, may even break a very small one.
Watching some of the tutorial videos I saw that roughing passes were done with the same bit as the finishing pass.
This is kind of hard to explain as the deference is mostly semantics. I had been looking at it wrong. I had been looking at Roughing Operation as a strictly chip clearing operation and the Finishing operation as a stand alone finishing cut. And it can work that way if you cut slow enough (increasing potential cut time 200% to 300%). But you can also treat the Finishing operation as more of a “Final Layer” of the previous operation by using the same bit (as implied in the error message). Slowing down on just the “final layer” to clean up any surface finish issues. (increasing potential cut time 10% to 20%)
Again this is more about my assumptions and expectations in how I approached setting up my cuts. Now that I better understand how the operations can work together I am hoping to get better results.

Yep - That was always the plan
Actually, I am planing on making these in several woods, sizes and styles and if I can, sell them, if not I will give them out as gifts.

Earwigger · March 3, 2016, 7:41pm

Interestingly, I have not run into that error. I typically always use a 1/4" FLAT endmill to do the roughing and then follow up with a ballnose. I did notice that the ballnose would often encounter cuts greater than its tooling settings. Hence, the decreased feed rate on the finishing pass. But then again, I never use smaller than a 1/8" ballnose, so never had any breakage.

Still, l’m looking forward to seeing more results.