Spindle speeds and feedrate cap

[HuFlungDung]

I just got ONEcncXP today.

In my usual style, I usually just poke around with stuff and see if I can make it work. To me this indicates how intuitive a program is. I usually read the help later on.

Verdict: you guys have really done an outstanding job of the post configuration setup. I run a Shadow controller, and this uses some of the most off-breed command language of all of them, and I think I have most of them set up already.

I did check the help index to see if it made reference to this next issue, but didn't see any reference to spindle or speeds.

Okay, now for a potential problem I would like to discuss: the material and tool lists are fine and dandy. But, I think that there should be a general parameter in NC setup that asks us for the maximum speed of the machine's spindle, and hopefully, a comparison could be incorporated so that if the machine is running flat out, that the maximum feedrate for a given tool in a given material, at this speed cap, would be automatically calculated and inserted in the program. This would be good for everyone.

Now as a side issue, my Shadow controller does not use direct rpm commands, but rather runs on a percentage of Max rpm, thus all my speed range commands are from 0 to 100. Is there any way to handle this kind of a speed command issue, by converting from actual rpm (as calculated from your material tables) into percentage for output into the gcode? This converted output would only need to appear when the gcode is created, and not within the tool setup when creating gcode. I was hoping that maybe you could add this option in the general tab/decimal options/spindle speed. FYI, the Shadow spindle commands are whole numbers only, no decimal permitted.

Now, back to exploring........

[HuFlungDung]

No one has any comments about this? Do all your machines have unlimited spindle rpm's available?

[wms]

Hu,
That's right my machines will turn up to 100,000 rpm and balance is no problem.

But seriously, I don't pay too much attention to what the cam system suggests for spindle speed and feeds.
I found I always want to "tweek" them anyway.
So when I'm going thru the tool path wizard I adjust the speed and feed to my liking.

I know in a perfect world it would be nice to have the system output the perfect speed and feed.
And if you get all the variables set up in the material sheet and tool sheet, it will output code based on those variables. But things like max spindle speed and the condition of the work piece and the way a person machines will "muddy" the water.

As for the spindle code needing to be a percent of max spindle speed. That's a new one to me. All my machines want an actual speed with no decimal point.
So I'm not any help here.

I guess I'm so used to "tweeking" my programs after post,(especially at tool changes) that I don't know any better.

We still have the problem of the "First" move to part at tool change where it always goes to xyz instead of xy at clearance then to z. (The safe way)

[HuFlungDung]

Originally posted by wms Hu, That's right my machines will turn up to 100,000 rpm and balance is no problem. But seriously, I don't pay too much attention to what the cam system suggests for spindle speed and feeds. I found I always want to "tweek" them anyway. So when I'm going thru the tool path wizard I adjust the speed and feed to my liking.

Yes, I can do that and we would all have to tweak. But, I am sure the intention of the programmers is to have a starting speed and feed that is theoretically correct. I've got one mill that runs at 2500 max and another running at 6000 max, so I think the effort to cap the speed at those figures and then adjust the feed according to the speed cap would be worth making, if the feature is incorporated within software at all. It is this exact lack of precision that has forced you and I to become the tweakers that we are

I know in a perfect world it would be nice to have the system output the perfect speed and feed. And if you get all the variables set up in the material sheet and tool sheet, it will output code based on those variables. But things like max spindle speed and the condition of the work piece and the way a person machines will "muddy" the water. As for the spindle code needing to be a percent of max spindle speed. That's a new one to me. All my machines want an actual speed with no decimal point. So I'm not any help here. I guess I'm so used to "tweeking" my programs after post,(especially at tool changes) that I don't know any better. We still have the problem of the "First" move to part at tool change where it always goes to xyz instead of xy at clearance then to z. (The safe way)

You have this Z problem? Hmmm, I know what you are referring to, but I don't see it. In your NC setup "Tool format" do you have a
G00 Z{CR}
inserted after, let's say, when your spindle turns on?
Here is a sample of the way my program would begin, including the first few lines of the toolpath.

G40
G75
G80
G90
X-4. Y0. Z1. G92
T2 (.375 INCH 3/8 CARBIDE BALL MILL)
F18.4569
S9228 M3
T200
/Z1. = (G00 Z{CR} in your NC setup Tool Format, /= G00 in Shadow)
/X0.6064 /Y-0.0952 /Z1.
/X0.6064 /Y-0.0952 /Z0.05
F9.2284
X0.6064 Y-0.0952 Z-0.1
X0.6202 Y-0.0489 I0.3627 J0.0023

[wms]

HU,
I was not disagreeing with you.
It would be great to have the things you talk about.
I'm as lazy as the the next guy and any thing to make my life easy I'm for.

About the z problem, I need to dig into the setup and get it set up to do as you say. I need a G43 z.1 h(t) in there.
This needs to be after the tool change and after the first move to position.(with no z movement)
Just haven't spent the time to get it just right.
I told you I was lazy.

[HuFlungDung]

WMS, what kind of machine config are you using?

For that line that you requested:
G43 z.1 h(t)
I believe this equals what I have to use for executing the tool offset in Shadow/Bandit which is simply:
T2 = the tool changer command
T200 = the tool offset executes.

Anyways, there is a lot of functionality built into the NC setup, and it takes a bit of trial and error to understand how to use it.
A few simple entries in the right place here = an entire script in bobcad.

[wms]

Hu,
Using the HAAS cfg.
Your right about the few line thing.
I guess I'll put down the remote and fix my problem as you have "shamed" me into it.
I also cleaned my PM up and cleaned my temp file now the Pm messages should be flying in.

[HuFlungDung]

Yes the new version fixes your decimal point in S parameter issue.

From your Tool format for Haas:
M5 G40 G49 G80
M9
({TDES})
{T} G43 {H} {D}
M6
{F} {S}
M3
{COOLANT}
G0 Z{CR} <--- added this


Got this for output. What do you think? You can try adjusting the Zero options before you post, too. That may have a favourable impact on your initial Z height. It seems to add on.

N90 G0 G40 G49 G80
N100 G0 G90 G54
N110 M5 G40 G49 G80
N120 M9
N130 (.375 INCH 3/8 CARBIDE BALL MILL)
N140 T2 G43 H2 D2
N150 M6
N160 F18.4569 S9228
N170 M3
N180 G0 Z1.
N190 G0 X0.6202 Y-0.0488 Z1.
N200 Z0.05
N210 G1 Z-0.1 F9.2284
N220 G3 X0.625 Y-0.0001 I-0.2468 J0.0488 F18.4569
N230 X0.625 Y0.0001 I-0.125 J0.0001
N240 X0.6202 Y0.0488 I-0.2516 J-0.0001

[wms]

Hu,
Thanks I'll give it a try.
Sorry I was downloading that file we talked about.

[wms]

Hu,
This what I came up with.
It's not exactly the way I want but real close.

Start lines
{T} M6 ({TDES})
G90 G80 G40 G55
{s} M3
G43 {H} / M8


End line

M01


Notes:
{T} M6 ({TDES}) = Tool number, tool change, tool description
G90 G80 G40 G55 = Reset canned cycles, set work offset
{s} M3 = Spindle speed, turn spindle on clockwise
G43 {H} / M8 = Set tool length offset, tool length number, block delete, coolant on

Works for me but I would like a way to make the first xy move after tool changes (at tool changer height) with no z move, then turn on tool length and then move to a safe z clearance.


The way it is now is if you put "Extra clearance" in the clearance plane, it will move there every time it goes to clearance.

[HuFlungDung]

WMS,

I was noticing the differences in the number of Z options offered in OnecncXP's drilling cycles, versus what you are offered in the mill pathing.

I wonder why they cut those out? It seems that the extra clearance height in the drilling options is just what we need to be able to use everywhere, not just in drilling.

What do you think? Compare the gcode output you get before a drill cycle with the output you get before milling.

Maybe this would be worth petitioning for if you find it will fill the need.

In my case, I used to use my controllers tool length offset option to serve as my "extra Z" option, ie., I would move to the start XY coordinate and then execute the offset, which my controller actually forces an immediate tool movement of the offset amount. This method is difficult to implement, too, because then I need to be able to insert that offset command after the first line of coordinate code has been generated. This is possible in the drill cycle setup, however, for regular milling, it is imperative to also have this tool offset command in the start line box, which in effect, give me two instances of the same command written into my gcode whenever I use a drill cycle.

[borrisl]

As a newbie, I would LOVE for a CAM application to ask me a few questions. Like: What spindle speed are you using? What type of material? You already include end mill size, so how about a little help on feed speeds? Great Idea, too bad I know very little about programing.