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

[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...m-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/ijnggmyv10...0PINE.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...m-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

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 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...m-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