tool parameters

[Anonymous]

Hey Fusion 360 Gurus,
New cnc router retrofit with Dynomotion KFLOP and KSTEP boards.

Selected a stock endmill but the G code had a G43 tool length offset.

Edited the tool parameters to ero offset.

Still showed up exactly as before.

Tried the emc.cps post processor.

The emc post processor results in several G codes that complicate the machine tool position.
Specifically, the G43 command for tool offset.
I manually load cutters in the spindle collet.
How does this tool offset get established?
Additionally, the G53 command references all dimensions to machine zero rather than the XYZ zero established manually to the part material.
How to remove tool offset parameter and use part material zero with absolute dimensions?

Or better yet, is there a post processor that will not use G43 and G53?
I need to reference XYZ zero from the part material surface. Not referenced relative to the machine zero.

I tried editing the tool with zero length offset. See excerpt at bottom.
G43 still has an offset value.

Thanks,
Ted

Th following excerpt is an example generated by Fusion 360 using the emc.cps post processor.

%
(1010)
(EMC POST)
(T5 D=0.25 CR=0.09 - ZMIN=0.318 - BULLNOSE END MILL)
N10 G90 G94 G17 G91.1
N15 G20
N20 G53 G0 Z0.
(ADAPTIVE2)
N25 M9
N30 T5 M6
N35 S5514 M3
N40 G54
N45 M8
N55 G0 X0.3815 Y-0.1865
N60 G43 Z2.0991 H5
N65 G0 Z1.6991

[skidsolo]

The tool length offset is a parameter in the controllers software, when the control reads the tool number and G43 the lenght in that parameter is applied to the Z position of the tool. Your program example includes a line with G54, this is the part origin that is again established through the contoller software to set the part zero. G53 is usually machine zero. The contoller software has work offsets from G54 to G59, this is for setting multiple parts to be cut each on thier own origin.

Move the machine to the position of the XYZ datum of the part on the machine, then use this in MDI mode to set the part origin on the machine G10L2Pn G10L2P1X0Y0Z0 (Set Fixture Offset #n)  P1 =G54 P2- G55 etc

[Anonymous]

skidsolo,

How does the Dynomotion KMotionCNC machine controller software know anything about a tool number in Fusion 360?

The Fusion 360 tool path viewer that simulated the result looks fine.

When viewed in the machine controller software KMotionCNC it has problems.

Code G91.1 specifically is not compatible and breaks the G Code listing.

I am looking for a post processor for Fusion 360 that will work without modification of resulting G Code for the KMotionCNC controller software.

How do we get post processor support from Fusion 360 support group?

Your quote follows:

"Move the machine to the position of the XYZ datum of the part on the machine, then use this in MDI mode to set the part origin on the machine G10L2PnG10L2P1X0Y0Z0 (Set Fixture Offset #n)  P1 =G54 P2- G55 etc"

This is not clear to me.

I viewed the tool path in the KMotion simulate run mode on the provided graphical screen.

The tool path plunged through the table with one post processor.

On another the tool path first came down to the material surface and then dragged across to an XY position.

Next it raised to the safe position and then started the tool paths properly.

Last it finished the tool paths and again dragged across the material surface and stopped at the XYZ zero, also at the material surface.

Please decode what you are trying to say with the last string of characters:

G10L2PnG10L2P1X0Y0Z0 (Set Fixture Offset #n)  P1 =G54 P2- G55

Cryptic string.

Please parse and explain steps.

regards,

Ted

[skidsolo]

This is from the kmotion webiste when the control reads a line with G43 it looks inside this file for the relevant fusion360 tool number then apply the length offset.

As for workfixture offsets (part origin) you need to move to the origin of the part on the machine get the tool you are using and get it on the center of the part origin in X and Y now move down in Z until it touches the part surface (you must make the top of the part in Fusion360 Z zero as well). Now make a note of the X, Y and Z coordinates and insert the

Lets assume the part origin is X 21.563 Y 16.325 Z-5.236 from machine zero G53

numbers into your G10 line.

to set G54 first coordinate syetm in the software Kmotion execute this line in MDI mode 

G10L2P1X21.563Y16.325Z-5.236

more info here

http://dynomotion.com/Help/KMotionCNC/GCodeOffsets.htm

Sorry its complicated but its just the way Kmotion CNC works, it very similar to how industry standard Fanuc contols work.

[Anonymous]

skidsolo,

I have established a homing routine that finds the X, Y and Z machine
limits and zeroes the machine.
Next in the process of setting up a job I manually install the cutter.
I then jog to the origin of the job material.
Usually the front left corner at the material surface.
I then zero the X, Y and Z axis on the KMotionCNC operator screen.
This action places the current location values into the G92 Fixture Offsets.
Why is it necessary to remember these origin values and insert them into
a G10 line?
I assume the tool path values will or should execute from this new zero
position.
However there is a 2 inch tool length coming from somewhere that will
either jump up 2 inches or drive into the table 2 inches.
I do not need the tool length to offset anything as I am using the
actual tool to set up the job origin.
Furthermore, since I manually install cutters the tool length is not a
constant in the collet.

Additionally, some of the post processors I have tried and viewed in
simulate mode use a G28 command to go to the machine limits and then
come all the way back to the current position to start the tool paths.
This is ridiculous to run all the way to limits every time you run a job.

What post processor to use that does not require this unnecessary motion?
Is there a specific G Code post processor in Fusion 360 that will run
tool paths without editing?
You have not stated which post processor to use.

Is there a way to edit a post processor to work directly with the
location of the tip of the installed cutter at the manually set material
origin?
How do you edit a post processor?

Where do we get post processor support for Fusion 360?

Lastly, has anyone at Fusion engaged the Dynomotion folks to collaborate
on a specific post processor?

regards,
Ted


---
This email has been checked for viruses by Avast antivirus software.
https://www.avast.com/antivirus

[skidsolo]

It seems you dont have to write anything down to set fixture offsets

Zero Using Fixture Offsets

Zero/Set Buttons near DROs allow the User to Set the DRO to Zero or a Specified Value.  This is accomplished by adjusting GCode Offsets.  When this option is selected then the currently selected Fixture Offset will be adjusted.  When unchecked the Global G92/G52 Offset will be adjusted.

It would help if you indicated the post processor you used, and the specifc changes you need. We dont use KmotionCNC, I am just reading their website..

[Anonymous]

skidsolo,
I am trying to determine which post processor to use to provide
edit-less functionality.
Perhaps you could download KMotionCNC to evaluate and suggest an
appropriate post processor.
Is there a tool or wizard to edit post processors?
Please advise,
Ted


---
This email has been checked for viruses by Avast antivirus software.
https://www.avast.com/antivirus

[skidsolo]

I have downloaded the software and will start testing.

[Anonymous]

skidsolo,

I appreciate the effort.

If a Fusion 360 user has a CNC machine that matches one of the post processors in the extensive list that is great.

However, it would be appropriate to provide a generic post processor, and a means to easily edit, for CNC machines not included in the list.

I understand the tool length offsets are used and needed for some applications with fixed tooling and tool changers.

Loading various cutters manually does not provide for this constant value.

Therefore, for these manual load systems a post processor that does not expext or provide a tool length offset would be helpful.

With the understanding that the operator uses a method that incorporates the cutter in locating the tool path origin on the material.

Is there a generic post processor that provides this functionality?

Regards,

Ted

[skidsolo]

I made a special post for you to drive the Kmotion software in simple single tool mode which is the default.

I removed all G28 G43 and G54-G59 commands and assume you are using G92 for the workpiece origin.

Without G28 and G53 at the end of the program, the tool will stay in the last posistion of the G code.

Please test and advise

[Anonymous]

Hey skidsolo,
I appreciate the effort.
What is the name of the post processor in the list?
regards,
Ted

---
This email has been checked for viruses by Avast antivirus software.
https://www.avast.com/antivirus

[Anonymous]

Hey skidsolo,

Below is the screen print of the list of post processors.

KMotionCNC.cps - RS-274D is not in the list.

Please advise,

Ted

[Anonymous]

Hey skidsolo,

Downloaded the attachment.

How to install?

Ted

[HughesTooling]

On a PC from your username.

Mark

[skidsolo]

click on the folder at the top of your screen shot copy that post configuration folder path into windows explorer, and paste the post processor file you downloaded into that folder.

[HughesTooling]

Once installed you need to select Personal Posts. 

Mark

[HughesTooling]

If you save to that folder I think it messes things up after an update.

Mark.

[Anonymous]

Mark,

The directory your screen print indicated was empty.

I copied the attachment file to it anyway.

Same result.

Does not show in post list.

[Anonymous]

Mark,

Selected Personal Posts and there it is.

Thanks,

I will test soon.

regards,

Ted

[Anonymous]

skidmoto,

In KMotionCNC if you check the simulate box and click the G Viewer tool you can see the cutter and the tool paths.

You can select one of several views and zoom and pan with the mouse and wheel.

If you check run it is super fast and shows the result of all tool paths.

However, if you click Single Step in the tool bar at the top you can see each command execute the move.

Unfortunately, in both cases the small image of the tool does not move and there are no tool path traces.

Unknown behavior.

Ted