Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

cylindrical engraving

Anonymous

cylindrical engraving

Anonymous
Not applicable

I am trying to engrave on a 1.5" piece of aluminum using my tormach a axis/4th axis 

 

Here is the file I'm trying to use as a test model to get the hang of things before beginning on the final product.

 

My first setback I encountered is that I cannot seem to select all of the letters when trying to select the models geometry

 

Does anyone know why the feed rates in my code are so high?

 

I've also been given an error in the previous try1 & 2 posts - missing feedrate was the warning in path pilot on the tormach.

 

I've attached the f3d file

 

I have toyed around with this for quite sometime but I am stumped

 

 

 

 

 

 

 

0 Likes
Reply
Accepted solutions (1)
2,808 Views
34 Replies
Replies (34)

Anonymous
Not applicable

yes, in the center of the part just like in the model/cam atmosphere

 

 

0 Likes

daniel_lyall
Mentor
Mentor

I am see that to


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

0 Likes

daniel_lyall
Mentor
Mentor

@Anonymous In this bit of code the part that is red is how it is now , I changed the first 0 to 1 and it post with the letters around the correct way with it being 0 it's mirrored.

 

I found the same thing with my own 4th axis post's

 

// Define Master (carrier) axis
masterAxis = Math.abs(rotary) - 1;
if (masterAxis >= 0) {
var rotaryVector = [1, 0, 0];  // was var rotaryVector = [0, 0, 0];
rotaryVector[masterAxis] = rotary/Math.abs(rotary);
var aAxis = createAxis({coordinate:masterAxis, table:true, axis:rotaryVector, cyclic:true, preference:1});
machineConfiguration = new MachineConfiguration(aAxis);

setMachineConfiguration(machineConfiguration);
// Single rotary does not use TCP mode
optimizeMachineAngles2(1); // 0 = TCP Mode ON, 1 = TCP Mode OFF
}

 

@xander.luciano Is this correct 


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

1 Like

Anonymous
Not applicable

@daniel_lyallNO Smiley Sad

 

Unfortunately this didn't work for me. I made the changes but I'm still getting backwards letters.

 

I have no idea what to do

 

 

0 Likes

daniel_lyall
Mentor
Mentor

OK For test to see if it's the post or pathpilot where the problem is.

 

The post you have been useing should not of had the problems with G01, So it could be something is wrong with the post.

 

Can you try the 2 posts attached the A- should work fine with the letters mirrored, The A+ should be bang on, These post were working when I did them in November.

 

You may only need the tcp changed from 1 to 0 this bit here line 134 and 135 

 

setMachineConfiguration(machineConfiguration);
optimizeMachineAngles2(1); // map tip mode

 

To work out if it's the post or pathpilot useing a post that is known to work is the best way forward.


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

0 Likes

daniel_lyall
Mentor
Mentor
Accepted solution

Here you go these should be good


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

2 Likes

Anonymous
Not applicable

Success, Bingo !  Post A-   (AMinus)  attached above is the correct post. Boom. super excited. Thank you so much for your help, Now if only I knew how to remove the g28 for x and Y at the end of the post...

 

 

Amazing work Xander and Daniel lyall

0 Likes

Steinwerks
Mentor
Mentor

@Anonymous wrote:

Now if only I knew how to remove the g28 for x and Y at the end of the post...

 


Have you tried changing useG28 to No in the post dialogue?

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

daniel_lyall
Mentor
Mentor

Why do you want that removed, 

 

Most times for safety reasons Have G28 is a good idea as it does this 

 

N16370 M9
N16380 G28 G91 Z0.  (Moving Z to a safe places before moving X and Y )
N16390 G28 X0. Y0.
N16400 M30

 

Not Having it like this If there is something in the path off the cutter it will hit it as it's moving all at once It will be a mistake/accident that you hit the object but it can happen

 

Haveing G28 G91 Z0 means the cutter will go up then X and Y will move harder to crash this way.

 

To turn it of in the pre post dialog you change it from yes to no Black arrow in pic.

 

G28 off.png


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

0 Likes

Anonymous
Not applicable

I don't know if I called the g28 in the correct context. but

 

turning off g28 in set up box will this effect the rest of the code or just the end?

 

this is the scenario I'm referring to:

when the cutting is all finished and the z does a g30 then x and y axis move all the way to the limit switch  (at the absolute end)

 

I don't want this to happen... 

 

 

In my opinion this more likely to crash something  

 

 

 

I just want the z axis to g30 and coolant shut off and spindle shut off but x and y stay where they were at the end no moving.

 

no more X and Y going to limit switch  

0 Likes

daniel_lyall
Mentor
Mentor

That's absolutely fine as long as your are aware that If you have a clamp or a fixture in the path of the machine going to Machine home (G53)  the G30 move (Your Machine zero postion). It can crash in the fixture/clamp.

 

It's uselessly fine if you rember to set the Clearances height in cam to above the fixture or clamp the red bit of code is.

 

it's set to go 18.9 mm above the 4th axis on my machine there is nothing for it to hit at 1 mm above the 4th axis, it's just so the the dust shoe does not break whats in the 4th axis.

 

If you turn G28 off the end code looks like this.

 

N34830 G1 X-47.464 Z31.1 A6.767 (end of cut)
N34840 G0 Z50. (move Z above work to the set Clearances height in the heights tab in CAM)

N34860 M9  (all coolant off)
N34870 M30 (move to machine 0)

 

Yes I am being a safety Nancy but it's for people who don't know what they are doing if they read this post. 


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

0 Likes

xander.luciano
Alumni
Alumni

Thanks @daniel_lyall for handling this over the weekend!

 

Just wanted to tie up the loose ends before submitting the issue and getting the Tormach PP updated. Looking through the PP you posted, I can see you properly flipped the rotary axis by using [-1,0,0] to create the axis:

 

var aAxis = createAxis({coordinate:0, table:true, axis:[-1, 0, 0], cyclic:true, preference:1});
machineConfiguration = new MachineConfiguration(aAxis);

 However, simply using -X in the properties instead of X should work:

 

// Define rotary attributes from properties
var rotary = parseChoice(properties.rotaryTableAxis, "-Z", "-Y", "-X", "NONE", "X", "Y", "Z");
if (rotary < 0) {
    error(localize("Valid rotaryTableAxis values are: None, X, Y, Z, -X, -Y, -Z"));
    return;
}
rotary -= 3;

// Define Master (carrier) axis
masterAxis = Math.abs(rotary) - 1;
if (masterAxis >= 0) {
    var rotaryVector = [0, 0, 0];
    rotaryVector[masterAxis] = rotary/Math.abs(rotary);
    var aAxis = createAxis({coordinate:masterAxis, table:true, axis:rotaryVector, cyclic:true, preference:1});
    machineConfiguration = new MachineConfiguration(aAxis);
    [...]
}

I'm also curious as to where Tormach needs the feedrate, since clearly this doesn't match up with the documentation. Does the controller actually require the feedrate on every line? If there were G02/03 arc movements, does it need the feedrates there?

I'm having NYCCNC take a look at the updated post, but it would help to confirm all this so that we (hopefully) solve all the issues at once.

 

Thanks a ton for the help!

-Xander Luciano


Xander Luciano
CAM Content Developer

If my post is helpful, press the Kudo button - If it resolves your issue, press Accept as Solution!
Quick Tips: When to resselect CAM geometry | Understanding Smoothing in CAM | Adaptive Facing | Online GCode Viewer
0 Likes

daniel_lyall
Mentor
Mentor

Yep I just got him to use what I know works.

 

from the tormach manual

 

7.5.2 Linear Motion at Feed Rate – G01 For linear motion at feed rate (for cutting or not), program: G01 X~ Y~ Z~ A~ F~

Word Definition

X~ X-axis coordinate

Y~ Y-axis coordinate

Z~ Z-axis coordinate

A~ A-axis coordinate

F~ Feed rate

 

This produces coordinated linear motion to the destination point at the current feed rate (or slower if the mill won’t go that fast). The axis words are optional, except that at least one must be used.

The G01 is optional if the current motion mode is G01.

If cutter radius compensation is active, the motion differs from the above; see Cutter Compensation later in this chapter.

If G53 is programmed on the same line, the motion also differs; see Absolute Coordinates later in this chapter.

 

It is an error if: •

All axis words are omitted

• G10, G28, G30 or G92 appear in the same block

• No F word is specified

 

Now the part that was failing and why

 

7.6.2.11 Feed Rate Mode – G93, G94 and G95

To set the active feed rate mode to inverse time, program: G93 Inverse time is used to program simultaneous coordinated linear and coordinated rotary motion.

In inverse time feed rate mode, an F word means the move should be completed in [one divided by the F number] minutes.

For example, if the F number is 2.0, the move should be completed in half a minute.

When the inverse time feed rate mode is active, an F word must appear on every line which has a G01, G02, or G03 motion, and an F word on a line that does not have G01, G02, or G03 is ignored.

Being in inverse time feed rate mode does not affect G00 (rapid traverse) motions.

To set the active feed rate mode to units per minute mode, program: G94 In units per minute feed rate mode, an F word is interpreted to mean the controlled point should move at a certain number of inches per minute, or millimeters per minute, depending upon what length units are being used.

To set the active feed rate mode to units per revolution mode, program: G95 In units per revolution mode, an F word is interpreted to mean the controlled point should move a certain number of inches per revolution of the spindle, depending on what length units are being used. G95 is not suitable for threading, for threading use G33 or G76.

 

It is an error if:

• Inverse time feed rate mode is active and a line with G01, G02, or G03 (explicitly or implicitly) does not have an F word

• A new feed rate is not specified after switching to G94 or G95 canned cycle return level – G98 and G99

 

So what you did to the post was a fix I will have a look at the direction change and fix that in the copy I have.

 

@Anonymous

To Get the machine to just goto a Z position When it's finished cutting just doing a G30 I am not 100% sure that it will do what you wont. I need you to test this.

you may be able to change it in pathpilot see below. unless @xander.luciano has some idea how to do it.

 

7.5.9 Return to Pre-defined Position – G30 and G30.1

G30 uses the values stored in parameters 5181 and 5183 as the X and Z final point to move to.

The parameter values are absolute mill coordinates in the native machine units of inches.

G30 makes a rapid traverse move from the current position to the absolute position of the values in parameters.

G30 X~ Z~ makes a rapid traverse move to the position specified by axes including any offsets, then makes a rapid traverse move to the absolute position of the values in parameters 5181 and/or 5183. Any axis not specified won’t move.

G30.1 stores the current absolute position into parameters 5181-5183.

 

It is an error if:

• Cutter Compensation is turned on

 

 

 

 


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

1 Like

xander.luciano
Alumni
Alumni

Thanks for posting the documentation, that helps a lot!

 

It is an error if:

All axis words are omitted

• G10, G28, G30 or G92 appear in the same block

No F word is specified


By the looks of it, seems to me that a feedrate is required for every G01 regardless of whether in inverse time or units per minute. In that case I need to add the line to both OnLinear() and OnLinear5D().

 

Can you post the documentation for Arcs also please? I'm curious as to whether G02/G03 need a feedrate on every line. I know that it is required for G93 - inverse time mode, but I'm not sure about G94 - units per minute feed rate mode.

 

Thanks for the info!

-Xander Luciano


Xander Luciano
CAM Content Developer

If my post is helpful, press the Kudo button - If it resolves your issue, press Accept as Solution!
Quick Tips: When to resselect CAM geometry | Understanding Smoothing in CAM | Adaptive Facing | Online GCode Viewer
0 Likes

daniel_lyall
Mentor
Mentor

I got it from here https://www.tormach.com/tormach-product-documents.html?doc_prod_name=PathPilot&doc_cat_name=Manuals

 

page 101 and 102 it does not say anything about a feed being needed.

 

the G01 does not need a feed in the post With the one he's useing now it does not have G93 or G94 in the code just a G94 at the start.

 

He did not say if he tested it with a G94 with no feed.

 

It worked with the F on a G93 and 94 and it was just inverted useing X- as the axis should fix that.

 

Are you going to johns tomorrow It would not be hard to test, it will only takes minutes if you just have a gcode to test with, done with no F on a G94 line. 

We know it works with A F on the G94 line.

 

 

If I had a tormach this would be easier.


Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz

Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn

0 Likes