Z lag (?) eats through my tabs and part - help!

[chairguy]

I have a 2014 PRS Alpha 96" x 48" that I'm going to use for two-sided 3D milling of hardwoods. I've run the leaf bowl sample file included with the machine and had no problem a few weeks ago. But now when I go to mill some chair legs, the Z seems to occasionally stick in low positions and ends up eating through my tabs half the time, only to pull up and back into correct position, then do it again somewhere else. (It may even dive down prematurely - I can't recall). It also eats through the part (chair legs) on occasion. I've tried recreating the cut files and even tried running from a different computer, but the mistakes happen in the same places, so this isn't random. Attached are photos showing my paths (side view) in Partworks 3D (looking down the side of the file, you can see all the way through the tabs, so the file seems correct.) But in the photo you can see how the 1/2" round nose roughing pass eats right through the occasional tab or chair leg, leaving the whole thing looking like swiss cheese. Anyone ever seen this before? Any ideas?

I'd be incredibly grateful for any help.

Thanks,

Kevin

[chairguy]

For some reason my attachments got reduced to something too small to see. Does anyone know how to load larger pictures on here?

[gc3]

if preview look correct then is a machine issue or how you are setting up material on table and setting up machine for toolpaths

[steve_g]

Kevin…
What are you using for a spoilboard? If it’s been a few weeks since you surfaced it, good chances are, if it’s MDF its absorbed moisture from the sir and swollen. The swelling happens in a non-uniform manner, It may be fine where you zeroed but not 5 inches away…
SG

[scottp55]

Kevin, Try converting to a .jpg about 1900X1200 or slightly smaller, that's about the limit for attaching.
scott

[Brady Watson]

Wood moves when it is being cut - especially solid wood. Some have a tendency to bow up as internal stresses are relieved (eating tabs) - in those situations tabs alone 'ain't gonna cut it' - so you need something else too.

Excessive speeds will cause the tool to run rough. What speeds are you running when you witnessed the tool 'self-correcting' ? This would be your MS speeds. (EG - MS,2,1) in your SBP 3D finishing toolpath.

-B

[chairguy]

Thanks everyone, although I apologize; I may not have described my problem so well.

Brady: After rechecking my Move Speeds and Ramp Speeds, I noticed that the settings that came programmed into the software weren't at their defaults (I was a bit surprised by this, as I would think when I load the software it would start with default settings). For each value below, the first number listed is where the setting was; the second number is their default, to which I reset the values:

[VS]
[S]PEED VALUES
XY Move Speed - 3 > 3
Z Move Speed - 3 > 1
A Move Speed - 2 > 1
B Move Speed - 50 > 50
XY Jog Speed - 14 > 12
Z Jog Speed - 6 > 3
A Jog Speed - 4 > 3
B Jog Speed - 100 > 100

[VR]
[R]AMP VALUES
XY Move Ramp Speed - 2 > .4
Z Move Ramp Speed - 2 > .4
A Move Ramp Speed - 10.16 > .4
B Move Ramp Speed - 10 > 10
XY Jog Ramp Speed - 2 > .4
Z Jog Ramp Speed - 2 > .4
A Jog Ramp Speed - 10.16 > .4
B Jog Ramp Speed - 10 > 10
Move Ramp Rate - 5.08 > .2
Jog Ramp Rate - 5.08 > .2
3D Ramp Threshold - 100 > 100
Minimum Dist to Check - .15 > .15
Slow Corner Speed - 65 > 65
KeyPad Ramp Rate - .2 > .2
Small Circle Def (OBS) - .25 > .25

I also ran a ground wire to ground the machine and dust hose as mentioned here (http://shopbotwiki.com/index.php?title=Grounding_your_ShopBot), to rule out static. (To ShopBot: Given the apparent importance of this step to Bot functionality, not to mention avoidance of sawdust explosions, it might be worth including this step and supplies with the initial installation process).

To my relief, resetting the Move and Ramp Speeds to the above defaults definitely took all the heavy jarring and jerking motion out of the cutting that I had experienced on my first two cut file trials (the 2D shopbot logo sample file, and the 3D leaf bowl sample file - both of which milled perfectly, even if the motion was jarring)....

...But resetting the Move and Ramp Speeds didn't solve the problem of the bit diving into the chair leg tabs or chair legs themselves. After reading more in the forum, I don't think I was losing Z, since most people speak of this term in the sense of the Z gradually slipping down. For me, the bit was occasionally ignoring movement commands in the Z and driving straight along the X axis (my tooling paths are oriented along the X axis), meaning that it would occasionally eat straight through my tabs or my part, which ever was in the path of the bit at the time. After eating it's way straight through (these gouges ran anywhere from a half-inch to 6 inches long), the bit would then pull back into correct position and continue as if nothing happened. Does this sound like a case of "missing steps"? When I re-ran the file on top of the botched part, the bit would make the same mistakes, gouging through the same places (So I guess that rules out static).

As a test, I reran the Leaf Bowl sample file, reducing the feed rates even further just to be extra safe, and although my first attempt at the Leaf Bowl worked fine, even if it was jarring, this second attempt at the Leaf Bowl retained the chair-leg problem of occasional gouging along the X. I've attached screen grabs of my settings, and will follow up with images of the the cut preview, actual cut results, and the Cut3D .v3D file itself (if you load the .v3d just make sure the bit info matches mine). Hopefully since this Leaf is a file everyone is familiar with, it will be easier to troubleshoot.

All help is tremendously appreciated, because I'm at a loss at this point.

[chairguy]

Here are those images of the cut preview and actual cut results.

[chairguy]

Hmmm... anyone know a good way to share a 10.4 Mb Cut3D .v3D file?

[ron_moorehead]

Drop Box works for sharing large files

[Brady Watson]

Your cut speeds are wonky. Change them to 2,1 and use that as a baseline for all 3 toolpaths. .4 and .3 IPS is just too slow for that part. It wants to go your target 2 or 1 IPS, but the Z is holding it back. Set it to 2,1 and it should eliminate the problem.

Go read towards the end of this article (or the whole thing if you are bored...) about speeds that the machine likes for 3D cutting: http://www.shopbotblog.com/2008/03/a-ramping-the-vr-command-and-how-to-tune-your-tool-for-maximum-performance/

Although you can use a ball end mill for both roughing and profile cutting - it isn't ideal. You want to use a square end mill for these. It will cut faster as well, so you can put your roughing stepover value at 40% and leave it. 5% for the finishing pass is too low. You're way into diminishing return below 7-8%. Use 10% as a baseline. By profile cutting with a ball, you'll have a tool radius on the bottom edge...unless you go 1/2 the diameter deeper than the thickness of the part.

I think adjusting your speeds will help or fix the issue...and the settings I mentioned should get you cutting quality at faster speeds. I am not sure why your tabs would be getting cut through - but I do know that if you don't have a setting correct in PW3D, this is possible. Re-check that you have "preserve tabs" checked and "material to leave" @ zero on the cutout toolpath.

Hope that helps. Let us know how you make out.

-B

[chairguy]

Thanks. This link will take you to the Cut3D .v3D file itself (if you load the .v3d just make sure the bit info matches ).

mine)https://www.dropbox.com/s/ijnggmyv10qo547/DEEP%208in%20LEAF%20BOWL%20IN%20PINE.v3d?dl=0

[chairguy]

Thanks again Brady. Does Onsrud make a 1/2" end mill? It seems like such a basic bit, but oddly, I couldn't find anything carrying that name. (does it go by a different name?).

I'll redo my settings as you mentioned above and will let you know how it goes!

[chairguy]

If anyone else is encountering problems with 3D cutting, here are the settings I'll be changing tomorrow:



In ShopBot 3:

Use all “default” settings: those listed on “PRS_Ramp Values.jpg” at http://www.shopbotblog.com/2008/03/a-ramping-the-vr-command-and-how-to-tune-your-tool-for-maximum-performance/

But change:

[VR] [R]amp Values
3D Ramp Threshold to 150
Minimum Distance to Check to .08
Slow Corner Speed to 25%-65% (but probably really 30%-45%) (lower percentage tells it to take corners slower; it eliminates or greatly reduces the tendency for the tool to ‘bang’ when it meets a sharp wall of a relief carving.
Fast Stop Threshold to .2 (from 3)
Keypad Stop Threshold between 1.75 and 2
Keypad Ramp Rate to .2 (for crisp movement with the arrow keys) or .8 (for precise small moves with the arrow keys)

[VS] [S]peed Values
Here are a few speed combinations I have found to work, without symptoms of the tool slowing down to wait for the Z axis: 2,1 – 2,2 – 3,2 – 3,3 – 5,3

[FP] [P]art File Load
Make sure “Preserve tabs” is checked when loading the tool path right before cutting



In PartWorks 3D:

Material Size & Margins
Change symmetrical machining margin to .6mm (larger than the diameter of my roughing bit) so roughing bit goes all the way down (not doing this is why my 1/8” bit broke… also because it was hickory).

Set “over cut distance below the cut plane” to the diameter of the bit to make sure no radius or “parting line” is left

Change Plunge Rate to 1ips on all tool paths

Roughing Use an end mill to rough, keep roughing stepover at 40%

Finishing pass stepover should be 10%

Set “material to leave” @ zero on the cutout tool path

Files that have a lot of surface or background texture will benefit from a higher 3D Threshold value, a lower Move Ramp Rate and a higher Slow Corner Speed. If you find that your tool sounds too rough for your liking, return the Move Ramp Rate to 0.2. If it is still happening, reduce the 3D threshold to 175 and if it is still happening, reduce the Slow Corner Speed. These settings have the most influence over 3D cutting. Additionally, since the Minimum Distance to Check also works in 3D, you may want to try lowering the value so that it is less sensitive to those little details in the background.



Saving Your Specialized Settings to Use at Another Time
OK, so you have your [VR] settings dialed in for perfect 2D cuts. You can type in the US command and save your configuration with a meaningful name, like ‘Brady2D.sbc’ and then move on to tune your tool for the type of 3D cutting that you do. You might want to save a configuration for V-carving and another for 3D relief cutting as well. After you have saved each configuration, you can easily call it up by typing in the UR command. It will ask you if you want to reset the current configuration. After affirming that this is what you want to do, you will see a list of configurations that you can choose to load, including the ones that you saved from your tuning sessions.For

[Brady Watson]

Kevin,
I didn't realize you are working in metric. It said you were from the US :rolleyes:

Make changes to your VR settings ONLY after you have changed units to Imperial/Inches if you are going to use my numbers. THEN switch it back to metric.

Speeds will need to be scaled accordingly. E.G. - Instead of MS,2,1 inches per second (IPS), your speeds should be represented as millimeters per second, which would be approximately MS,50,25. Speeds need to be set within the tool database in PW3D per toolpath, not using the VS command in SB3.

'Preserve Tabs' setting is in PartWorks3D on the cut out toolpath tab, not SB3.

-B

[chairguy]

Thanks Brady - you're very generous and meticulous with your advise.

Sorry - I am actually working in inches: that .6mm was a typo and should have been .6".

Not sure if you saw my small post: any idea if Onsrud makes a 1/2" end mill?

If I change my Feed and Plunge Speeds to 2 and 1 (respectively) in PW3D, do my SB3 XY Move and Z Move Speeds not need to change to match these?

When loading the toolpath into SB3 right before cutting, do I need to change any of the parameters on in the [FP] [P]art File Load fill-in sheet (attached)? (Do I need to turn Tabbing to "1-on" or change any other settings?)

[Brady Watson]

You're welcome.

No - You can ignore that fill-in sheet. In 15 years - I've changed things on that screen only once or twice in the thousands of files I've run. Just hit enter when you see that screen and blow past it.

Onsrud sells router bits for routing. They don't sell end mills, per se. Aside from a little chip-breaker curl on the very tip of a 2-flute upcut spiral router bit, it is absolutely identical in every way to a 2-flute solid carbide end mill. The difference in price between an Onsrud 2-flute tool and a premium quality 2-flute end mill is substantial.

I've been using end mills for woodwork & general CNC cutting after making the comparison in grind between the two early on. I get my end mills from Oberg Brothers (http://www.obergbrothers.net/) because they sell top quality lines @ a discount. I run end mills instead of 'spiral router bits' because it is a source of contention for me...as if router bit companies purposefully jack up the prices on 'pretty spirals' for 'stupid woodoworkers' - so I'll never buy a spiral upcut router bit again if I can help it. Downcut spirals are different...

A 2-flute carbide end mill is pretty much your bread and butter as far as cutting tools go. Aside from this, a spiral-O flute is another 'cuts just about anything' grind that can pretty much be used on anything, including metals, woods and plastics. Onsrud makes several excellent tools of the O-flute variety including straights and multi-fluted ones.

If there's one thing I've learned over the years, it is not to use 'cheapie' bits or end mills. A quality tool will outlast the cheapie by a wide margin. This has a lot to do with the quality of carbide used, but more importantly, the 'micro-grain' size used to make the blank. The smaller the grain, the longer it will last...carbide hates heat. When it overheats, it ejects little 'cubes' of carbide from the surface. The smaller the grains, the less of an effect on the geometry of the tool, especially at the cutting edge, which means it stays sharp longer.


-B

PS - PDFs require downloading. JPG/JPEG would be easier for people to see. If your pics are too large, you can download the Windows Image Resizer and right-click on pics to resize them pretty easily...

[chairguy]

Fantastic. Just wrote to Oberg Bros to see what they'd advise for a 1/2" end mill for hardwoods (ideally with a 5" total length since I'll be running some thick blocks of wood eventually).

As far as O-Flutes, the ShopBot Starter Bit Kit came with an Onsrud 65-025 1/4” - SC 1F Upcut Spiral O Flute... guessing this is what you were talking about?

Thanks also for the advise on the image loading and recommendation to ignore the file load fill-in sheet.

One last thing: If I change my Feed and Plunge Speeds to 2 and 1 (respectively) in PW3D, do my SB3 XY Move and Z Move Speeds not need to change to match these?

[Brady Watson]

Obergs should be able to give you what length tools are available in a given diameter. So...You should know diameter and the cutting edge length you want + number of flutes, which will mostly be 2.

Yes...that weird looking single flute spiral is an O-flute.

When you run a part file it supercedes the move speeds set in SB3 temporarily and then reverts to them when the files is done.

-B

[chairguy]

PROBLEM SOLVED!... whatever it was. Thanks Brady!!

So here's the final summary of what I did to fix the gouging that was happening in the X direction:



In ShopBot 3

Use all “default” settings: those listed on “PRS_Ramp Values.jpg” at http://www.shopbotblog.com/2008/03/a-ramping-the-vr-command-and-how-to-tune-your-tool-for-maximum-performance/

But change:

[VR] [R]amp Values
3D Ramp Threshold to 150
Minimum Distance to Check to .08
Slow Corner Speed to 25%-65% (but probably really 30%-45%) (lower percentage tells it to take corners slower; it eliminates or greatly reduces the tendency for the tool to ‘bang’ when it meets a sharp wall of a relief carving.
Fast Stop Threshold to .2 (from 3)
Keypad Stop Threshold between 1.75 and 2
Keypad Ramp Rate to .2 (for crisp movement with the arrow keys) or .8 (for precise small moves with the arrow keys)

[VS] [S]peed Values
Speeds here will be superseded by whatever feed rates and plunge rates are entered in PW3D part file’s tool data pages.

[FP] [P]art File Load
Don’t bother changing anything on the fill-in sheet right before the file loads to the machine



In PartWorks 3D

Material Size & Margins
Change symmetrical machining margin to 0.6” (larger than the diameter of my roughing bit) so roughing bit goes all the way down (not doing this is why my 1/8” bit broke… also because it was hickory).

Set “over cut distance below the cut plane” to the radius of the bit to make sure no radius or “parting line” is left

All Toolpaths: Change Feed Rate to 2ips; change Plunge Rate to 1ips (based on this advise: “Here are a few speed combinations I have found to work, without symptoms of the tool slowing down to wait for the Z axis: 2,1 – 2,2 – 3,2 – 3,3 – 5,3”)

Roughing Toolpath: Use an end mill; keep roughing stepover at 40%

Finishing Toolpath: Pass stepover should be 10%

Cut-Out Toolpath: Set “material to leave” @ zero; make sure “Preserve tabs” is checked


I also:
1) uninstalled and reinstalled PW3D and SB3 software.
2) closed all other programs and internet/WiFi
3) shut down windows then OSX and restarted everything, keeping all other programs closed

[Brady Watson]

3) shut down windows then OSX and restarted everything, keeping all other programs closed

SB3 is not designed to work on OSX. I am not sure that using a dual boot setup, and using Windows that way to run SB3 is a hot idea. There could be some issues with this, especially with the USB drivers and Apple hardware, but if it is running OK for you - then great. This will probably change as things move forward, but officially it is only supported via Windows on a PC laptop or desktop CPU.

Glad you got it sorted. Thanks for reporting back.

-B

[chairguy]

I began running SB3 and PW3D on my Mac through Parallels, but it was supposed to be temporary, as I had a new dedicated PC on the way. But once I started running SB3 from the PC, the program would get stuck "thinking" (unresponsive arrow cursor with spinning wheel) very often, and I find programs on PC's take longer to restart, so I went back to using my Mac (SB3 still stalls like this on the Mac occasionally, but less often it seems, and recovering/reloading is quicker). Is this SB3 stalling normal?

[Brady Watson]

Is this SB3 stalling normal?

No. Not at all. You really don't want to minimize the importance of a good computer that has only the bare essentials installed on it. It is literally an extension/part of the CNC controller itself - not just a GUI/front end.

Avoid Dell machines...and the el cheapo ones like eMachines. CL has deals as well as refurbs via NewEgg.

-B