Public Service Announcement - Make More in Less Time via Tuning

I machined about 20 3D reliefs over the past 2 days and I wanted to share my findings, because they are significant. I was running v3.8.14 on it, if for no other reason than it's been a cold Winter & I just didn't get around to updating it. I was having some issues when starting a file (it would pause too long/hang once in a while) so it was time to load up v3.8.26. I installed it and by mistake did a UR (was going for UI when brain fart happened) - setting my machine settings back to stock. I continued machining my reliefs - except instead of taking 17 minutes, they took 20 min each.

So, I opened up the VR settings and tweaked the defaults a little & re-ran the file. This resulted in a time of 16 min. So I went back and tweaked some more & got the time down to 12 min(!) - Absolutely no changes in the toolpath or move speed. Everything was untouched in the SBP. (4.625 x 2.5" part, 3D raster @ 10% SO, 1/16" ball, MS,2,1; 18k, cherry)

The first round I changed the 3D Ramp Threshold from 100 to 150, my usual custom 'tweak'. This alone knocked off 4 minutes or 20% of the overall time. The 2nd adjustment, I changed my Min Dist to Check from .15 to .08 (my usual default tweak number) AND the 3D Ramp Threshold from 150 to 200...this brought my ET down to just over 12 minutes, or a savings of 40% over the original ET! Yowsa! :cool:

So that meant that I was able to machine 5 parts per hour compared to only 3 parts per hour with the original VR settings. After a while I get sick of seeing the same thing being machined over and over again...so this was a real blessing! If you have no clue what I am talking about when I mention VR, go read this article.

I usually recommend that people only tweak the Slow Corner Speed setting from the default 65 to something in the 35-50 range, as this will change the characteristics of the tool enough to understand what is going on. You have to be careful fooling with some of the settings, as they will cause the tool to move in unexpected or undesirable ways. For the most part, you aren't going to hurt your tool...you can always click back to default settings at the bottom of the VR fill-in sheet.

3D Ramp Threshold adjusts the tool's sensitivity to ramping conditions. Higher values result in more aggressive cutting moves, with less cushion in all directions. If you are running a cat whisker diameter bit, you might want to leave this down around 100-150. You won't find any love above 400.

When I run files, I always use FE to look at it before I run it. I almost always tweak the MS to be what I want it to be & maybe program the tool to goto a location off the material when done. I will often open up the VR settings and adjust the Slow Corner Speed if I find that the tool is taking corners too fast or not fast enough. SCS works in the XZ & YZ planes as well...so keep that in mind.

As I've said before, the machine will go as fast as it wants to go or as fast as the material and bit will allow you to go...so be prudent. I've listed speed recommendations for cutting 3D in the article.

Play around...be patient, listen to the tool and what she wants...coffee helps. The more you can learn about your tool, the better you will be as a machinist & the more free time you'll have to play. :p

Have fun!

-B

Thank you Brady, you are a gentleman and a scholar. I appreciate your knowledge and willingness to share.

Jim

Thanks Brady!!
scott

Thank you Brady.

I always read your posts. Ya darn right time is money!

Can you give us a few pics to go with your description? I would like to see some of your 3D production machining.

Dave

I tuned my machine for tight corners and short runs (probably 90% of my work) after reading Brady's article a few years ago. The difference was incredible. These days I have three separate config files that I load depending on what the makeup of the sheet I'm working on is. It's worth spending as much time as you can reading about and understanding the various settings as you'll get that time back ten fold if not more.

All - You're welcome.

Dave - No pics at the moment...I just ran them off without taking any. Nothing too fancy - plinth blocks in a starburst/fan pattern.

-B

Quote:

---

Originally Posted by Brady Watson

I machined about 20 3D reliefs over the past 2 days and I wanted to share my findings, because they are significant. I was running v3.8.14 on it, if for no other reason than it's been a cold Winter & I just didn't get around to updating it. I was having some issues when starting a file (it would pause too long/hang once in a while) so it was time to load up v3.8.26. I installed it and by mistake did a UR (was going for UI when brain fart happened) - setting my machine settings back to stock. I continued machining my reliefs - except instead of taking 17 minutes, they took 20 min each.

So, I opened up the VR settings and tweaked the defaults a little & re-ran the file. This resulted in a time of 16 min. So I went back and tweaked some more & got the time down to 12 min(!) - Absolutely no changes in the toolpath or move speed. Everything was untouched in the SBP. (4.625 x 2.5" part, 3D raster @ 10% SO, 1/16" ball, MS,2,1; 18k, cherry)

The first round I changed the 3D Ramp Threshold from 100 to 150, my usual custom 'tweak'. This alone knocked off 4 minutes or 20% of the overall time. The 2nd adjustment, I changed my Min Dist to Check from .15 to .08 (my usual default tweak number) AND the 3D Ramp Threshold from 150 to 200...this brought my ET down to just over 12 minutes, or a savings of 40% over the original ET! Yowsa! :cool:

So that meant that I was able to machine 5 parts per hour compared to only 3 parts per hour with the original VR settings. After a while I get sick of seeing the same thing being machined over and over again...so this was a real blessing! If you have no clue what I am talking about when I mention VR, go read this article.

I usually recommend that people only tweak the Slow Corner Speed setting from the default 65 to something in the 35-50 range, as this will change the characteristics of the tool enough to understand what is going on. You have to be careful fooling with some of the settings, as they will cause the tool to move in unexpected or undesirable ways. For the most part, you aren't going to hurt your tool...you can always click back to default settings at the bottom of the VR fill-in sheet.

3D Ramp Threshold adjusts the tool's sensitivity to ramping conditions. Higher values result in more aggressive cutting moves, with less cushion in all directions. If you are running a cat whisker diameter bit, you might want to leave this down around 100-150. You won't find any love above 400.

When I run files, I always use FE to look at it before I run it. I almost always tweak the MS to be what I want it to be & maybe program the tool to goto a location off the material when done. I will often open up the VR settings and adjust the Slow Corner Speed if I find that the tool is taking corners too fast or not fast enough. SCS works in the XZ & YZ planes as well...so keep that in mind.

As I've said before, the machine will go as fast as it wants to go or as fast as the material and bit will allow you to go...so be prudent. I've listed speed recommendations for cutting 3D in the article.

Play around...be patient, listen to the tool and what she wants...coffee helps. The more you can learn about your tool, the better you will be as a machinist & the more free time you'll have to play. :p

Have fun!

-B

---

Is this something you could talk about at the McGrew camp please??

Quote:

---

Originally Posted by Ajcoholic

Is this something you could talk about at the McGrew camp please??

---

Well...I'm supposed to talk about 3D digitizing, but we can certainly talk about this on the sidelines. Scanning is applicable to all users. This is applicable to SB owners only, since other controllers regulate ramping differently. With there being a mix of different CNC brands at the camp, I'd lose attention pretty quick for those that don't have a blue machine.

-B

Everything Brady is saying is true. Tuning makes a big difference when it comes to production. For one offs it's not a big deal, who cares if it takes 16 minutes instead of 14 minutes? But when running production, a few minutes here and there add up quickly. Altering your cut file to accommodated better tuning and keeping and loading different settings depending on the job you are about to run is a great way to find some time.

I took one job that required about 31 minutes to run a sheet. I redesigned the file to eliminate some of the smaller radiuses and tuned the ramp settings specific to the job and it now runs in just over 22 minutes. Huge difference when you run 10 sheets, almost 90 minutes saved! Well worth the effort. If I try to run other jobs with those settings the machine "bangs around" too much. If I run this job with standard tuning it takes about 25 minutes. But being able to alter my cut file combined with the allowed improved tuning paid off big.

Thanks Brady,

I will give this a try, was cutting a Chip/Dip bowl this weekend and the corner cuts was so slow that the bit looks black at the tip, guess that is the issue (hope so anyway).

Quote:

---

Originally Posted by barrowj

I will give this a try, was cutting a Chip/Dip bowl this weekend and the corner cuts was so slow that the bit looks black at the tip, guess that is the issue (hope so anyway).

---

Probably. The best thing would be to reset your VR to default via the fill-in sheet to make sure other settings didn't get messed up. I don't know why, but some people's settings get jacked up for one reason or another, through no apparent fault of their own. It's always good to take a peek and check your settings.

Unless it is a very specific/exotic job, I only mess with the Slow Corner Speed, Min Distance to Check and 3D Ramp Threshold. It is rare, and usually unnecessary to mess with the other settings, but there are times where you need to.

Oh...VERY IMPORTANT: Be sure that your MS is set to something reasonable when machining. So if you are hogging out a 4x4" pocket for a bowl, it is not possible to run this job at 6" per second. Maybe 2" per second is more reasonable because of the accel/decel ramp. It will only be at 2 IPS for a very short distance before it needs to slow down to move in stepover & raster back again the other way.

If you set your speeds too high (MS), then the tool can get choppy and erratic as it tries to compensate for poor choices in MS. You cannot go by speed values in ANY CAM software - they are just defaults with NO logic behind them. I cannot tell you how many times I have trained someone only to find they were running v-carve toolpaths at the default MS,6,6 - because they thought those were recommended speeds. This is not so!

You can observe the effects of improper MS values for yourself as an experiment to get greater understanding. Put an obscene MS value in for XY to cover a small area (say a pocket in a 4" square space @ MS,6,1) and leave your VR @ default settings) An 'air cut' above the table is fine for this. No need to actually cut. Observe the movement of the tool & maybe even place your hand on one of the gantry end plates and feel what is going on. Then pull your MS back to like 1.5 or 2 IPS for XY and hear/feel the difference. There will be some variation in effectiveness from one model to another, but you should be able to pick up on "do's & don'ts" with this.

-B

Brady,

I had the speed set at ms 2,.5 and was using a 1/2" bit to do the rough pocket and as it would do the 1"-2" half circle it would seem to crawl at (just as an example) .1 or .2 then jerk up to 2ips. I cut this same item before upgrading my communications card and SB3 3.6.46 and it was fine. I was also using the Shopbot arc file you sent me a few weeks back but even changing that didn't seem to matter. My slow corner speed in VR is 65 .

The tool can't go 2 IPS within an area of 2" (assuming 1/2 circle with dimensions of 2x1") with a 1/2" bit. This means that the largest straight line distance would be only 1.5" using a 1/2" bit. 2.00" minus 0.5" = 1.50"

-B

Brady,

It really is a bigger project than that, I've attached a copy of my crv file so you can see what I am working with. If 1/2" is too big to rough this, please let me know.

Thanks,

Joe Barrow
joe@joebarrow.com

http://www.joebarrow.com/download/xmas-bells.crv

Joe,
I don't see any problem with that shape aside from the 1" circles where it may slow down a bit. Where are you getting the burn marks specifically?

-B

Thanks for the info Brady, thats what makes this forum great, I spend more time on the mechanicals and my designs, I forget about tweeking the controls.

Brady,

It's occurring in the arc/ 1/2 circle's and really slows to a crawl and just starts smoking then pulls out of the arc and cuts normal. I appreciate the help, really appreciated.

Joe

Thanks Brian.

Joe,
Post a screenshot of your VR settings.

-B

Brady,

As requested, I have not made any changes, still learning this but hope to learn lot's more at the Aspire camp in SC.


http://www.talkshopbot.com/forum/att...id=24408&stc=1

Sorry for jumpin' on Brady's thread here, but you need to reset your ramp values to default settings. The reason it's slowing down so much in the corners is due to the xy ramp speed of 0.1. Default is 0.4. A slow corner setting of 65 will also contribute to it. Try dropping that down in increments of 5 to see the results.

On a side note here, depending on what version of SB3 you are using (older versions had this problem), clicking on the 'reset' in the corner of the fill-in page may or may not set the actual defaults for your machine. I have seen it set values that are completely off, which may be the case here. You are better off to use UR and choose the default config file for your machine.

For anyone that takes the time to tune your ramp settings, take the time to also save out those settings so you can easily return to them at any time. You can do this with US to save the file. Open that file and edit it so that all there is in the file is the VR line and save as a .sbp or .sbc. You can then set up a custom cut that loads this file any time you want to use those settings. As an example, I have custom cuts to load various 3D ramp settings, various v-carve ramp settings, and my preferred default ramp settings all from the 'Cuts' menu.

No problem Scott - 2 heads are better than one most days :D

Yep...that .1 setting means that the tool will start moving from a dead stop @ .1 IPS. It makes the acceleration ramp longer than it needs to be for the kind of cutting that you are doing. On some setups it can cause COM problems because of timing between the Windows clock and the on-board SB processor if it is too low. This is why there is a step divider option for those who understand what it can do...

-B

Thanks Scott,

I am using SB3 3.6.46 and have not made any modifications to the defaults. I used the default settings for my machine (2005 PRT Alpha) so I'm sure some tweaking is in order.

Joe

Make your VR look like the attached pic.

-B

Thanks again Brady, I'll make the changes and try tomorrow and let you know the results.

Thanks Brady! This thread is worth bumping up to the top! I do production signs and just changed my settings, what a difference in completion time with absolutely no loss in detail!

Is the pic Brady posted up there with his settings the ones that shave off time?

Safe for me to plug in those numbers?

What will happen if I vcarve and profile cut with this?

Quote:

---

Originally Posted by Davo

Is the pic Brady posted up there with his settings the ones that shave off time?

---

No. The VR setting fill-in sheet I posted are my baseline numbers. Through hours of testing, I have found these to be good everyday settings that make the tool perform well. They are less aggressive than stock. They will make any SB run a little better overall, in the name of quality and machine smoothness.

Quote:

---

Originally Posted by Davo

Safe for me to plug in those numbers?

---

Yes. You will not hurt anything & can go back to stock settings by clicking the Reset link on the VR fill-in sheet.

Quote:

---

Originally Posted by Davo

What will happen if I vcarve and profile cut with this?

---

Your tool will run a bit smoother, although there are additional tweaks that can be made for small delicate carvings to minimize vibration at the tip of the V.

The whole idea of posting this thread is to make operators aware that in a production setting, you can gain more throughput by making small adjustments. It is imperative that you read my VR article on the main SB site in order to gain a proper understanding of what each setting does, as well as the logic behind it. Without knowing what you are doing, it would be like randomly turning screws on a carburator without knowing what each does.

It is possible to make the tool perform faster/more aggressively or slower and smoother depending on your needs. There is no one-size fits all because there are different adjustments in each situation - including the shape of the part being cut. If in production it would behoove you to test parts at various VR settings (using the methods described in my article) to see how much quality, speed or both you can gain by tuning. Otherwise, my settings listed above will work fine for general use.

-B

Thanks for the information, looking fwd to testing it out

Currently I spend about 1-1.5 hrs doing a 12" 3D piece with 2.5ips as the speed, and that's with 10% step over

Seems long to me

It depends on the level of detail and diameter of bit being used. 1.5hrs is wicked fast for a relief with a lot of detail requiring a 1/16 or 1/32" ball. It is all relative...and when all is said and done, the machine will go as fast as the material and design will permit.

-B

I use 1/8th tapered ball nose

I can only image the time it would take with a 1/16

1/32 is hard for me to imagine no snapping in a split second

1 to 1.5 hrs for a 12" 3D sounds really fast to me. The major speed constraint with a relief is the movement of the Z axis. There's only so fast you can move a piece of metal like that up and down. The X and Y movements have to take into account the speed of the Z so even if you upped the XY feed rate you wouldn't necessarily see a decrease in time.

so I'm doing pretty good on time then

How would this work when running Part Works V2.5 ?