MAX Speeds for PRT Standard??? (NO 4G)

[tuck]

Folks, I have an old PRT Standard 48 x 96, upgraded years ago from a PR with a new (at the time), control box, version 3.53. It's the beige colored control box that looks like a computer tower.

Ok, recently the little old computer I used to run the Bot out in the shop went belly-up on me, so I implemented another computer after downloading and installing the right software onto it (3.4.27). I had issues with Unit Values and called Shopbot for help and spoke with a really good guy named Christian. During the course of trying to straighten everything out, it came to light that I had my Z speed set @ .250 (1/4") ISP (raise & plunge). Christian asked me, "Why so slow?" I replied that it was the speed I had always used, having been told (before the upgrade) that anything faster was too fast and unreliable. Christian said, and I quote; "Oh no, Mark. You can set your Z speed to a lot faster than that now,...at LEAST 1.00 ISP!" Wow, I didn't know that! I guess that when I upgraded, I just figured I was getting a better and more reliable control box, not realizing that I could possibly cut FASTER! :confused:

I feel like a dummy, but then,...I obviously am a dummy. Ok, I admit it!:cool:

My question is for you Shopbotters that have the same set-up as I do. What are you using in IPS (Inches Per Second) for MAX reliable cut speeds, Z speeds, and jog speeds? I realize that hardness and thickness of materials is relevant. I'm mostly cutting 1/2" Ultraboard (foam board) these days, which is soft as butter.

I do NOT have the 4G! This is strictly standard.

What have I been missing????

[gc3]

max will be for xy 6ips z 3ips jog/cut...with 3.4.27

spend the $ for the 4g upgrade and don't look back 2K steps vs 200 per revolution

have a older PR with a PRT Z and can jog at 10-12 ips xy no issues and have done larger 3d carvings at 6ips xy 4ips z with great results

plus you can use latest software

but hey i am still new at this.....whadda i know

[tuck]

max will be for xy 6ips z 3ips jog/cut...with 3.4.27

spend the $ for the 4g upgrade and don't look back 2K steps vs 200 per revolution

have a older PR with a PRT Z and can jog at 10-12 ips xy no issues and have done larger 3d carvings at 6ips xy 4ips z with great results

plus you can use latest software

but hey i am still new at this.....whadda i know

Haha! You know more than I do Gene! Thank you for your prompt reply!

OH MY GOD! All of this time I have been poking along with 1/4" I.P.S. Z and 2.5" I.P.S. X,Y and jog! OH MY GOD! I AM AN IDIOT!:eek: It was about 7 years ago that I purchased the upgrade from the PR version and like I said, I just thought I was simply buying a more "reliable" control box and don't remember ever having been told of the faster speeds! 6 ISP cutting? 10-12 ISP jogging? 3" ISP Z? ARE YOU KIDDING ME? :eek: WOW!
The 4G upgrade would be out of my price range right now (times are kinda tough), but I will heed your advice when times are better. But I have read on these boards in the past that the 4G came with a lot of problems and also read where Shopbot doesn't even offer it anymore. Not true? I don't know.

Thanks again, Gene!

6 I.P.S.?

Captain Kirk: "Scotty, more power!"

Scotty: "Captain, I'm giving her all she's got!" :D

[Brady Watson]

On a 3G PRT, here are my recommendations*:

Max XY Speed when cutting = 2.5 IPS, 3 IPS if cutting low density foam
Max Z speed = 1.5 IPS, 2 IPS in foam

Denser material will require more torque & MS should be lowered accordingly. Adjust VR settings. Lower Slow Corner Speed to 40 to prevent lost steps when doing 3D by cushioning moves.

Max XY Jog Speed = 5** IPS
Max Z jog Speed = 3 IPS

*All rates should be lowered 0.5 IPS less than suggested if 'rolling heavy' with a big spindle (Colombo 5hp) and/or 5' wide tool.

**You can command the tool to go 6 IPS. However, it is impossible for the tool to go any faster than around 4.5 IPS. If you don't believe me, get the stopwatch out, command the tool to go say 30" at whatever speed you want, and do the math...The only 3G tools that would do nearly 6 IPS were plasma machines with 36T pinions...

-B

[tuck]

On a 3G PRT, here are my recommendations*:

Max XY Speed when cutting = 2.5 IPS, 3 IPS if cutting low density foam
Max Z speed = 1.5 IPS, 2 IPS in foam

Denser material will require more torque & MS should be lowered accordingly. Adjust VR settings. Lower Slow Corner Speed to 40 to prevent lost steps when doing 3D by cushioning moves.

Max XY Jog Speed = 5** IPS
Max Z jog Speed = 3 IPS

*All rates should be lowered 0.5 IPS less than suggested if 'rolling heavy' with a big spindle (Colombo 5hp) and/or 5' wide tool.

**You can command the tool to go 6 IPS. However, it is impossible for the tool to go any faster than around 4.5 IPS. If you don't believe me, get the stopwatch out, command the tool to go say 30" at whatever speed you want, and do the math...The only 3G tools that would do nearly 6 IPS were plasma machines with 36T pinions...

-B

Thank you BW. Actually, 3 I.P.S. cutting this ultraboard will be an improvement and just fine, but the biggest help will be the (much) faster Z speeds. I'm cutting pre-printed logos that are relatively small, with an average of maybe 60 of them on a 4 x 8 sheet of ultraboard. 1.5 to 2" I.S.P. for Z (vs. 0.250") will speed things up tremendously, not to mention the possibility of 5 I.S.P. jog!

OH MY GOD! After all this time, I am fixin' to discover unknown universes! I'm gonna go where I've never gone before! :D

Edit to say,...I don't do any 3D work and don't want to! Everything is 2D or 2.5D. I have the software for 3D, but I've never had any demand for 3D products.

[Brady Watson]

Mark,
Just keep in mind that the artwork, material and bit ultimately tell you how fast you can go. You certainly wouldn't want to cut a bunch of small letters or engraving at 2 IPS.

I would definitely save for a 4G upgrade and buy sooner than later...like all things, it may not be available forever.

-B

[MogulTx]

Yeah- and don't get TOO much speed envy. I was running a PRS Standard with PC Router- up until last month, and I ran my foam cut outs at about 4IPS every time- so it is not that much different.

Of course I was running a SINGLE pass at .75" deep and using a 1/2" DC Spiral and leaving nothing but an onion skin in the material... So it was "working hard" - if you can call cutting foam working hard.

I ran the "new" PRS Alpha the same speeds last night... with an HSD Spindle a 4HP, and 12,600RPM. It cut pretty nicely and I probably do not need to do much as far as adjusting the programs. What I noticed is that I was halfway through the second series of cuts before I realized that I did not have my hearing protection on! AMAZINGLY quieter operation. The noisiest thing in my shop is the dust collector right now.

I may start fiddling with the speeds and feeds. I need to figure out the dang chip calculator thing first!


Anyway- back to the topic of my post: Don't get TOO envious of speed. The greatest benefits I see in the Alpha is a greater accuracy and a MUCH quieter machine. (And more expense!)

Upgrade when you can, you will at least get some incremental speed and technology that will be supportable for a longer period of time!

[Brady Watson]

I need to figure out the dang chip calculator thing first!

Grassroots method of chipload calculation: Sight - Sound - Smell

How does the cut look? Clean edge? (good) Burned? (Going too slow, or tool is shot) Rough? (increase RPM) Does scrap side look better? (change direction - Climb vs Conventional)

How does it sound? Labored? (increase RPM) Screaming? (Reduce RPM)

How does it smell? Can't smell anything? (good) Smell burning? (bit dull or RPM too high)

Chipload is NOTHING MORE than the size of the chip coming off of each flute of the cutter. You want the LARGEST chip you can get off of your material WHILE maintaining good cut quality. If you took the dust foot and rooster-tailed the chips coming off of the bit into your hand, and then measured the thickness of the chip...THAT'S YOUR CHIPLOAD!

In many cases it is IMPOSSIBLE to run suggested chipload. The design itself could be too intricate to maintain 'constant contouring', which is just a fancy way of saying 'turn off all ramping' - since the tool needs to slow down in corners. Also, your hold down method may be too weak to allow ideal CL to be run because the force of the bit against the workpiece is too strong. Also, you may need to run at a lighter chipload in order to run a super long bit that will deflect or break if run at ideal CL...

I never use a chipload calc...I might look at the manufacturer's suggested range just to get me in the ballpark, but the tool and design has the ultimate 'say' on correct speeds. It's a lot like cooking...It'll TELL you when it is done...just as the CNC will tell you when it is laying down some sweet cuts or if it is hacking your beautiful material to shreds...

-B