Direction change lines issue milling hardwood

This forum is for general discussion about Aspire

Direction change lines issue milling hardwood

Postby marbles » Sun Nov 04, 2018 1:57 pm

Hi,

I’m trying to work out how to improve the surface finish in hardwood on these small terrain models, see pics below. For a first milling these 90mm models in hardwood theres plenty which is ok, however i’m wondering where to make improvements and which area to look at first. This is milled on a newly finished 4x4 cnc router build, which has linear rails and a 2.2kw spindle and is plenty stiff enough to mill 18mm ply so doubt that the mechanical side of things is an immediate issue.

From the pictures its clear the 90 degree direction change is showing as slight groove. Thats something I need to correct. I could change the material limits boundary from the square perimeter to a circular or curvilinear perimeter which would mean there aren’t any sharp corners. However cutting 90 degree corners should be well with the machines capability. The burr fur that noticeable can be address by changing the direction I guess.

Is this a problem that needs to be addressed in Mach3 first (I have CV set to on) perhaps it should be decelerating into and out of tight corners?

Perhaps in Aspire I need to slow down and/or only use a raster strategy at two different angles?

model size 90 x 90 x 20mm
material cherry

Finish pass
2mm ball end
120000rpm
feed 1800mm/min
plunge 900mm/min
stepover 9%

material limits boundary
set to material boundery

machine area strategy
set to offset, climb cut

Any suggestions greatly received. Thanks

P1120574.JPG

P1120573.JPG

P1120567.JPG
marbles
Vectric Apprentice
 
Posts: 21
Joined: Tue Jun 18, 2013 7:48 pm
Model of CNC Machine: homemade

Re: Direction change lines issue milling hardwood

Postby mtylerfl » Sun Nov 04, 2018 2:38 pm

My first thoughts are I would be using 8% stepover but that might not be the major cause of the visible lines (only a contributor).

I’ll bet it is mostly due to slight material movement. This occurs pretty much no matter what and can result in the line passes becoming more visible in spots. Also, make sure you have a flat spoilboard surface and the router is perpendicular to it. You’ve got to have everything “going for you” when raster carving.

“Fuzzies” can happen at any time. Grain direction and cutting direction can cause this. It’s common for raster carving but different woods are more (or less) prone to this. I always tell folks that’s what sandpaper is for (although that’s kind of a smart-alec comment).
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3284
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Direction change lines issue milling hardwood

Postby marbles » Sun Nov 04, 2018 2:57 pm

Thanks for thoughts.

I'd removed almost all the excess material with a step down rough cut so there was little material for the ball end to remove and little resistance for block to move.

There's a chance that this problem starts with a velocity or acceleration issue in Mach3 motor tuning. It possible its just running to fast into the corners, to jerky.

Sandpaper can pretty much fix 99% issues :)
marbles
Vectric Apprentice
 
Posts: 21
Joined: Tue Jun 18, 2013 7:48 pm
Model of CNC Machine: homemade

Re: Direction change lines issue milling hardwood

Postby martin54 » Sun Nov 04, 2018 3:13 pm

How much testing & tuning did you do once you had the machine built? Mach3 can take a bit of setting up to give the best results & as there are so many differences between machines when it comes to homebuilt then using someone elses settings doesn't mean that is whats best for your particular machine :lol:

What other 3D carving has the machine done & how do those results compare with these?
Are you using a straight 2mm bn or a tappered bit & what sort of length is it? Tool deflection could be causing some of this especially with a long narrow bit, stepover for me is generally trial & error, anything from about 10% down to 3% depending on size & material :lol: :lol:

You could try using a vector boundary & setting the vector larger than the finished piece if you are having problems where the machine changes direction, you might also want to look at your acceleration/deacceneration settings in mach as well

If fuzzies aren't bad then I generally don't worry to much about them, most of the time a stiff brush gets rid of them, on a terrain map then they might actually enhance the appearence :lol: :lol: :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3986
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Direction change lines issue milling hardwood

Postby marbles » Sun Nov 04, 2018 3:49 pm

Thanks for reply,

Machine Testing
I’ve been 3D carving large blocks of foam on my first 4x4 mach3 build for years but this is one of the first 3D test on the new build, carving wood. TDF i've had the same issue with grooved corners on the first machine but usually from running it too fast. I’ve copied over some of the settings and it could be that I just need to go through a series of tests to determine the limits. It may be that I have to make a different profile in Mach3 for carving smaller parts as opposed to the high speed for carving in 1200x 200mm blocks in foam I am used to. I also think either the acceleration of velocity in Mach3 is set too high and could do with a longer ramp up and down. Bit of research required to understand whats needed.

Bit
I used 2mm ball end. 6mm shank 30mm long straight bit with about 8mm usable flute. It was only cutting 1mm into the material but yes there could be deflection. Tapered R0.5mm ball ends on route from China.

Vector offset
Indeed on a revision to the job I set the vector larger to a larger area to see what would happen. What I can also do is set the machining limit boundary to a different selected vector that is circular or irregular this avoiding any sharp corners.
marbles
Vectric Apprentice
 
Posts: 21
Joined: Tue Jun 18, 2013 7:48 pm
Model of CNC Machine: homemade

Re: Direction change lines issue milling hardwood

Postby LittleGreyMan » Sun Nov 04, 2018 4:42 pm

marbles wrote:Bit
I used 2mm ball end. 6mm shank 30mm long straight bit with about 8mm usable flute. It was only cutting 1mm into the material but yes there could be deflection. Tapered R0.5mm ball ends on route from China.


I doubt you had deflection with these parameters. But no doubt a tapered bit will be a better choice.

Was the bit new and sharp?

How did you hold your material on the table? Wood moves a lot, so it has to be firmly hold.
Best regards

Didier

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 846
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: Direction change lines issue milling hardwood

Postby marbles » Sun Nov 04, 2018 5:34 pm

I used a new 2mm ballend. Difficult to tell how sharp it was, it wasnt blunt through.
Material held down with two metal bars screwed through to the table bed below. Cant be 100% but it felt secure. A slightly different factor, which I really hope is not the case is the transfer of vibration from the top of the Z down to the tip of the endmill. Its a 700mm Z axis, see pic.

What I think is likely is that I need to slow the machine down at corners either in CAM or Mach3...

Pic taken before final wiring completed..
axis.jpg
marbles
Vectric Apprentice
 
Posts: 21
Joined: Tue Jun 18, 2013 7:48 pm
Model of CNC Machine: homemade

Re: Direction change lines issue milling hardwood

Postby scottp55 » Sun Nov 04, 2018 5:59 pm

I'm betting on Machine/Mach 3/hold down issue for my 2 cents.
I've done a few topos, and have tried 2 different methods(but did NOT have Tiny Chinese TBNs at the time, so because I love detail, and my pieces are generally small I used Onsrud 30degree Engraving bit with a .01" flat at the time...looking forward to topos with the little TBNs:)
First method was VERY conservative as had not used Claro Walnut before.
Drillman1's .125" Downcut was used for roughing leaving .02".
Then used a 50/50 mix of Tung/Citrus thinner, and babysat dry spots for 30 minutes before wiping all excess off.
Cut 24 hours later against the grain, at IPS 1,1,18K and it came out good.
Second method in Cherry(pic is mis-labeled:( ....
Attachments
T4 RUN ROUGH PASS...LEAVE .02INCH SKIN.jpg
T5 SLATHER ON THINNED TUNG OIL.jpg
T7 WIPE EXCESS WAIT 24 HOURS 2.jpg
T10 66PERCENT DONE.jpg
T9.8.jpg
Last edited by scottp55 on Sun Nov 04, 2018 6:14 pm, edited 4 times in total.
User avatar
scottp55
Vectric Wizard
 
Posts: 2351
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Direction change lines issue milling hardwood

Postby scottp55 » Sun Nov 04, 2018 6:07 pm

Was the same exact model and bit(VERY sharp and pretty new!).
CEL is .5" on this bit, so model height was .45".
NO prep or rough cut.
Cut against the grain at same feeds and speeds, and it came out well.
I use small stepover (10% BUT ENGRAVING BITS ARE DIFFERENT! as it's a percentage of the FLAT).
With Chinese TBNs I plan on my first one to be about 4% for the trial cut at 1,1,16K.
No sanding on either topo pictured, just a rough(stiff boar bristle) brushing, and then a shoe shine(horsehair) brush.
scott
Attachments
9.1.16 Sully MDI Maple front 33 percent North side.jpg
9.1.16 SULLY MDI BLOWN OFF AND BRUSHED.jpg
User avatar
scottp55
Vectric Wizard
 
Posts: 2351
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Direction change lines issue milling hardwood

Postby Tailmaker » Sun Nov 04, 2018 6:29 pm

Given that the ripples are mostly a short distance behind the 90 degree-turn, I am wondering if there is some machine vibration due to the sharp turn, which could be reduced by smoother acceleration. But if that is true, it may be more efficient to stiffen up the gantry or frame.

I did not find "offset" a good strategy for such 3d-surfaces, since the surface texture does depend on the direction and there will be a difference no matter what. Long smooth strokes across the entire board will surely improve it and get rid of the 90 degree turns anyway. As for fuzzies, just make sure to go along the grain or across. At an angle I always get fuzz and tear-out.
Tailmaker
Vectric Apprentice
 
Posts: 153
Joined: Sun Jun 16, 2013 4:40 am
Location: Pasadena, CA
Model of CNC Machine: Home Built 4-axis Router

Re: Direction change lines issue milling hardwood

Postby marbles » Sun Nov 04, 2018 6:32 pm

scottp55 wrote:Was the same exact model and bit(VERY sharp and pretty new!).
CEL is .5" on this bit, so model height was .45".
NO prep or rough cut.
Cut against the grain at same feeds and speeds, and it came out well.
I use small stepover (10% BUT ENGRAVING BITS ARE DIFFERENT! as it's a percentage of the FLAT).
With Chinese TBNs I plan on my first one to be about 4% for the trial cut at 1,1,16K.
No sanding on either topo pictured, just a rough(stiff boar bristle) brushing, and then a shoe shine(horsehair) brush.
scott


Nicee geo pieces very nice and good strategy stats. Engraving bits is totally new to me but good to know. Thanks!
marbles
Vectric Apprentice
 
Posts: 21
Joined: Tue Jun 18, 2013 7:48 pm
Model of CNC Machine: homemade

Re: Direction change lines issue milling hardwood

Postby marbles » Sun Nov 04, 2018 6:49 pm

Tailmaker wrote:Given that the ripples are mostly a short distance behind the 90 degree-turn, I am wondering if there is some machine vibration due to the sharp turn, which could be reduced by smoother acceleration. But if that is true, it may be more efficient to stiffen up the gantry or frame.

I did not find "offset" a good strategy for such 3d-surfaces, since the surface texture does depend on the direction and there will be a difference no matter what. Long smooth strokes across the entire board will surely improve it and get rid of the 90 degree turns anyway. As for fuzzies, just make sure to go along the grain or across. At an angle I always get fuzz and tear-out.


I'm going to run some test tomorrow and play with the motor tuning in mach3 and set up new profile just for these smaller carving jobs and see if that makes a difference.
marbles
Vectric Apprentice
 
Posts: 21
Joined: Tue Jun 18, 2013 7:48 pm
Model of CNC Machine: homemade

Re: Direction change lines issue milling hardwood

Postby marbles » Sun Nov 04, 2018 7:00 pm

scottp55 wrote:Was the same exact model and bit(VERY sharp and pretty new!).
CEL is .5" on this bit, so model height was .45".
NO prep or rough cut.
Cut against the grain at same feeds and speeds, and it came out well.
I use small stepover (10% BUT ENGRAVING BITS ARE DIFFERENT! as it's a percentage of the FLAT).
With Chinese TBNs I plan on my first one to be about 4% for the trial cut at 1,1,16K.
No sanding on either topo pictured, just a rough(stiff boar bristle) brushing, and then a shoe shine(horsehair) brush.
scott



Was just looking again at your last image of the finish pass and the detail is very good! So this was done with a Onsrud 30degree Engraving bit with a .01" flat, right? Trying to work out what you mean by IPS 1,1,18K (i'm metric). Can you give me a breakdown of the feeds and speeds, if you have to hand..
marbles
Vectric Apprentice
 
Posts: 21
Joined: Tue Jun 18, 2013 7:48 pm
Model of CNC Machine: homemade

Re: Direction change lines issue milling hardwood

Postby martin54 » Sun Nov 04, 2018 9:37 pm

Was just looking again at your last image of the finish pass and the detail is very good! So this was done with a Onsrud 30degree Engraving bit with a .01" flat, right? Trying to work out what you mean by IPS 1,1,18K (i'm metric). Can you give me a breakdown of the feeds and speeds, if you have to han

It doesn't really matter what units you work in the software will work it out for you :lol: :lol: :lol:

Select IPS & then type in the value that Scott gave, then just select what ever metric units you are use to & the value will change to the metric equivelent :lol: :lol: :lol:

Your machine is completely different to Scotts though so don't expect his settings to give you the same results :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3986
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Direction change lines issue milling hardwood

Postby ger21 » Sun Nov 04, 2018 9:57 pm

This is milled on a newly finished 4x4 cnc router build, which has linear rails and a 2.2kw spindle and is plenty stiff enough to mill 18mm ply so doubt that the mechanical side of things is an immediate issue.


Don't be so sure.

A slightly different factor, which I really hope is not the case is the transfer of vibration from the top of the Z down to the tip of the endmill. Its a 700mm Z axis, see pic.



I think that's a very good possibility. Why is the gantry and Z axis so tall? All that height just makes the machine more flexible.

I also think either the acceleration of velocity in Mach3 is set too high and could do with a longer ramp up and down.


Generally, the only reason you would need to lower acceleration is due to a lack of rigidity. Higher acceleration **should** make the machine smoother, and more accurate, unless the machine is flexing.

As others have mentioned, I'd change the toolpath to raster back and forth, and never change direction over the workpiece.
Gerry
ger21
Vectric Wizard
 
Posts: 1199
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Next

Return to Aspire - General

Who is online

Users browsing this forum: BalloonEngineer and 30 guests