Plunge rate

[IslaWW]

Jason...
I agree, most DIY guys have gone with Mach3, especially years back when it was one of few available. Now days you can buy UCCNC and a good matched BOB for the same or less than mach3 costs. About 1/10 the bugs and much more modern control options. FYI, they have been working on Mach4 for almost a decade, and it doesn't appear that it will be sold as a DIY offering.

ShopBot, like all branded CNC's, even most DIY projects, are all built to a spec based on a price point. All mfgrs have big ones and small one, fast ones and slow ones, etc., etc. Same goes for TV's, trucks and anything else we want to buy. There is no one size fits all.

[TReischl]

I hate to say this, but the fact is that Aspire does control the feedrate, and it does set it to the Z feedrate when using the ramp/spiral function when profiling, witness the following code which was generated for Mach 3:

N19X0.0000Y0.0000F200.0
N20G00X-3.4026Y-3.1875Z0.2500
N21G00Z0.0000
N22G1X-1.3193Z-0.0401F50.0
N23G1Y-1.1479Z-0.0794
N24G1X-3.4026Z-0.1195
N25G1Y-3.1875Z-0.1587
N26G1X-1.3193Z-0.1989
N27G1Y-1.1479Z-0.2381
N28G1X-3.4026Z-0.2782
N29G1Y-3.1875Z-0.3175
N30G1X-1.3193Z-0.3576
N31G1Y-1.1479Z-0.3969
N32G1X-3.4026Z-0.4370
N33G1Y-3.1875Z-0.4762
N34G1X-1.3193Z-0.5164
N35G1Y-1.1479Z-0.5556
N36G1X-3.4026Z-0.5957
N37G1Y-3.1875Z-0.6350
N38G1X-1.3193F200.0
N39G1Y-1.1479

I had Z feed set to 50, and X,Y set to 200.

Most of us never notice the limiting Z feed thingy because we are not doing deep enough cuts on Z to allow the axis to reach very high feedrates. However, a few years ago I discovered it when doing some deep (4 inch) bowls and learned to pay attention to that Z feed when doing deeper work.

Those saying that "modern" controllers will go through all sorts of gymnastics need to consider that the controller works with the last F word that it was given. I have not seen anywhere on any machine or piece of software where one can spec an XY feed and a different Z feed. It probably exists somewhere, but I have not seen it.

Edit: Yes, one can spec XY feed and Z feed in Aspire, but the control only has one F word, obviously when Z is moving Aspire gives preference to that feedrate. Which is a very good thing.

[JasonDorie]

This is a 5 degree ramping profile, traversing a circle. Tool parameters are 100ipm feed rate, 30ipm plunge rate:

Code: Select all

N190X0.0000Y0.0000F100.0          - this is the XY feed rate (100ipm)
N200G00X6.0000Y1.8750Z0.2000
N210G1Z0.0000F30.0                - this is the plunge rate  (30ipm)
N220G1X5.9641Y1.8752Z-0.0031
N230G1X5.9281Y1.8756Z-0.0063      - the plunge rate continues through the ramp...
N240G1X5.8921Y1.8764Z-0.0094
N250G1X5.8560Y1.8775Z-0.0126
<snip>
N810G2X2.4445Y3.9086I2.0480J3.5807F100.0  - back to the proper feed rate
N820G2X1.8753Y5.9499I3.5555J2.0914
N830G2X1.8750Y6.0000I4.1247J0.0501

So apparently I'm not crazy. It does this if you choose a full spiral profile too. Basically, for the duration of the "plunge" part of the move it uses the plunge rate, and the lateral cut uses the feed rate, which makes total sense for a vertical plunge, and no sense for a ramping one.

[IslaWW]

Ted...
Thanks, you've just proven my point. Yes, Aspire is placing the "F50" command, via its postp, in that code you posted. That said, it (the feed callout) is there because that's what the controller specs call for. Look at some of the other posts in the postP folder.

A good number of the more modern versions will allow the XY to cut at the set 200 ipm rate as long as the Z plunge rate is not exceeded. That would use the 200/50 or 4:1 (25% slope) rule. If that ratio was exceeded, then the XY would move at the fastest speed that it could without exceeding the Z feedrate. Only in the case of a 100% slope: 1 to 1 or (100% slope) or 45* plunge would the XY actually slow to that of the Z.

As you might notice that code is reminiscent of old days hand coding or "single sticking" which only placed code that was changed in a given line, making code much easier to generate by hand. Modern design programs, such as we get and take for granted have many features built in to them to make good machining a lot easier to achieve than the ol guys did by using brute force at the keyboard.

EDIT: Add Jason to the list, thanks.

[IslaWW]

As a quick add... a 2" dia circle posted with a spiral toolpath 1" per rev. I will guarantee that the XY feedrate runs @ 100 ipm here, just as set.

[JasonDorie]

I think I see what's going on - On yours, the postP dictates the XY speed and the Z speed for feeds, then just outputs G0 or G1 codes. For Mach3, it outputs a feed value per move (G0 or G1), and in that case Aspire is just outputting the raw feed or plunge number.

So your version is allowing the machine to interpret the speed as it sees fit, whereas mine is forcing the machine to a set speed. What I want is the ability for Aspire to compute that ratio of allowable XY to Z speed and output the proper rate accordingly.

[IslaWW]

Jason...
Aint gonna happen with mach. The post outputs feed calls as per the controller specs. Now you know why most controllers went away from "the old way".

At the very least many, even most of the modern controllers, and especially the high end industrial stuff, allows the programmer or operator to set proper feeds and feeds. Using multiple feeds, even for all 6 axis at a time, is one of those things that modern controllers have evolved into.

Please understand that not all controllers will do what WinCNC will do, and not all machines are capable of <500msec acceleration to full speed, but when you have both....

By the way, I am not the guy that's here to tell people things they aren't sure if they should believe, I'm here to show you:

[JasonDorie]

I get that Aspire controls the rate, I was saying, as an option, they could alter that output rate to handle the mix between plunge and XY based on the slope. Mach just listens to the GCode. The math is trivial.

Here's mine doing rapid hole-cutting for halftones - I wrote the app that creates the GCode to drive this:


It does a rapid move down to zero, then a feed move to the hole depth, then rapids to the next hole position, and so on. It looks more like a sewing machine. Seriously - there's nothing preventing Aspire from doing this.

[FixitMike]

No app required. In the Material setup, set Z2 to a small value, like .01". The plunge moves will be made at the horiz. feed setting to .01" above the material surface, and then proceed at the plunge rate.

[Adrian]

Make sure you have RAPID_PLUNGE_TO_STARTZ = “YES” in your PP to enable that feature of rapid plunging to Z2.

[JasonDorie]

I noticed that when I was digging through the post files this evening - had never seen that before either. Going to have to dig through these a little more. Thank you!

As for the app, I wrote that about 6 years ago. VCarve / Aspire don't do so well when you hand them 36,000 circles to cut. The app can take a ton of shortcuts because it knows that's all they are.

[FixitMike]

Make sure you have RAPID_PLUNGE_TO_STARTZ = “YES” in your PP to enable that feature of rapid plunging to Z2.

Am I correct to assume it goes somewhere here in my PP? Did I put it in the right place?

+---------------------------------------------------
+ Commands output for rapid moves
+---------------------------------------------------

begin RAPID_MOVE

"[FC]"
"G00[X][Y][Z]"

+---------------------------------------------------
+ Commands output for the plunge move
+---------------------------------------------------

begin PLUNGE_MOVE
RAPID_PLUNGE_TO_STARTZ = “YES”
"[FP]"
"G1[X][Y][Z]"

[Adrian]

It should go at the top of the PP with the POST_NAME, UNITS etc.

[TReischl]

This is a very informative discussion.

Thanks for posting that code Isla, I was wondering how the control was getting two feedrates registered, obviously the F word followed by either XY or Z flags the control to determine each setting. Neat.

I have not had any problems doing spiraling as long as I remember to set the Z feed on the tool screen to the feed rate I want. I can see where doing an interpolation between two values would be handy and would negate my having to tax my aged old brain to remember these sorts of things. But maybe that is good, keep my grey matter from decaying prematurely.

These types of things illustrate just how messy writing CAM software can get.