issues with gcode file produced from fusion 360 used in mach3

recently downloaded fusion 360 and trying to design and output gcode to use in DIY 3 axis router controlled by mach3. I elected the wcs with z axis pointing up, x pointing to right, and y axis to 90 countclock to x
The model orgin was lower left top corner., My router and 600mm y movement, 500mm x movement and 90mm of Z movement. both the x and y home negative, but z since zero represents top
of gantry and bottom is negative, it homes positive. When I load the gcode into mach3 software and commence a run, I get a software limit error. Being new to all this, I have tried both using
"in computer" and "in control" for tool compensation. Both appear to generate a block of G43 code that wants to raise the z axis enough to provoke z axis softlimit error. I use a touch plate and
until I feel more comfortable usually trick the z axis to be 2 inches off actual work surface for purpose of air cut. I do select the mach3mill post processor to create the gcode. since I am new
to this whole process have a couple of questions. I work in MM in cad/cam and mach3..

Do you have a choice of letting fusion 360 by "in computer" tool compensation to simply load the gcode and and let mach3 follow the instructions which include he tool offsets without doing
any tool assignments in mach3.

Can the G43 command be remarked out or does this represent an elevation prior to rapid move to commence cutting

All indications are that I have my Z axis configured correct with zero at top, and -88mm at bottom of gantry travel ?

Any help with any of this would be greatly appreciated.
Anthony

I normally set all the heights in Fusion from the model (work) top. Your Z home position should be well Z positive from the work top, and everything below the work top should be Z negative. Check your heights in Fusion.

Could be something simple. 90mm Z movement is quite short.
Soft limit error might be the Z trying to go upwards first (safe Z)
An area in the code where retract height is higher than Z top limit depending on your tool height itself.

I also had soft limit errors in the beginning too.
Stupid question but 'home' and soft limits are related to 'machine' 0.0 coordinates and your parts are related to 'work' 0.0 coordinates. 2 different things alltogether. Have you definately got it right?
This was my problem.

Quote:

---

Originally Posted by kansaswoodrat

recently downloaded fusion 360 and trying to design and output gcode to use in DIY 3 axis router controlled by mach3. I elected the wcs with z axis pointing up, x pointing to right, and y axis to 90 countclock to x
The model orgin was lower left top corner., My router and 600mm y movement, 500mm x movement and 90mm of Z movement. both the x and y home negative, but z since zero represents top
of gantry and bottom is negative, it homes positive. When I load the gcode into mach3 software and commence a run, I get a software limit error. Being new to all this, I have tried both using
"in computer" and "in control" for tool compensation. Both appear to generate a block of G43 code that wants to raise the z axis enough to provoke z axis softlimit error. I use a touch plate and
until I feel more comfortable usually trick the z axis to be 2 inches off actual work surface for purpose of air cut. I do select the mach3mill post processor to create the gcode. since I am new
to this whole process have a couple of questions. I work in MM in cad/cam and mach3..

Do you have a choice of letting fusion 360 by "in computer" tool compensation to simply load the gcode and and let mach3 follow the instructions which include he tool offsets without doing
any tool assignments in mach3.

Can the G43 command be remarked out or does this represent an elevation prior to rapid move to commence cutting

All indications are that I have my Z axis configured correct with zero at top, and -88mm at bottom of gantry travel ?

Any help with any of this would be greatly appreciated.
Anthony

---

A G43 is not your problem it is what is before the G43 that is the problem cut and paste the start of the program here and we may be able to see what is going on from that

G43 is you Z axis work Offset just as G54 is your X and Y work Offset

Quote:

---

Do you have a choice of letting fusion 360 by "in computer" tool compensation to simply load the gcode and and let mach3 follow the instructions which include he tool offsets without doing any tool assignments in mach3.

---

That option doesn't affect Z. That compensation will decide whether G41/G42 is applied to the tool radius . You probably aren't using G41/G42.

The work offset on a 3 axis machine G54 (55 56 etc) has a x y and z component. Assuming the Z part origin is at top of the stock simply touch tool at top of stock and set G54 Z to zero.
For a machine without a tool changer or repeatable tool lengths this is the easiest method. G43 calls a tool length compensation, that length is in a tool table. On the simplest type of machines there's no need for this. However if you don't want to create a separate part program for each tool things get more complex.

Quote:

---

Can the G43 command be remarked out or does this represent an elevation prior to rapid move to commence cutting

---

Using the method I outlined above G43 can be deleted from the gcode file. In case you get tempted to hand edit the Mach3 post processor be aware your changes will be overwritten every time Fusion updates. There are ways to prevent the overwriting described in the fusion forums.
Edit/ To clarify:
G43 Z0.6 H1
can be edited to simply:
Z0.6

Will regenerate the gcode and try later today...thanks

I change the G54 to G56 and identify that location on mill somewhere near center of mill bed for nubie safety.

(SERVO_MOUNT_ADAPTER)
(FIRST FUSION 360)
(MACHINE)
( VENDOR HOMEMADE)
( MODEL DIY)
( DESCRIPTION GENERIC 3-AXIS)
(T1 D=3.175 CR=0. - ZMIN=-10.525 - FLAT END MILL)
N10 G90 G94 G91.1 G40 G49 G17
N15 G21
N20 G28 G91 Z0.
N25 G90

(BORE1)
N30 M5
N35 T1 M6
N40 S25000 M3
N45 G54
N50 G0 X5.404 Y52.667
N55 G43 Z16. H1

No question is stupid...been there done that. Anyway, yes I do know the difference. I use G56 and locate it somewhere near the
center of mill bed for nubie safety. I also change the gcode from G54 to G56. Once I jog the mill to desired position with G56 offset
selected, I zero x and y, they using touch block set z. One of the responses I have got spoke of making everything reference
from work top....am going to try that...hopefully will help resolve limit errors.

Quote:

---

Originally Posted by kansaswoodrat

I change the G54 to G56 and identify that location on mill somewhere near center of mill bed for nubie safety.

(SERVO_MOUNT_ADAPTER)
(FIRST FUSION 360)
(MACHINE)
( VENDOR HOMEMADE)
( MODEL DIY)
( DESCRIPTION GENERIC 3-AXIS)
(T1 D=3.175 CR=0. - ZMIN=-10.525 - FLAT END MILL)
N10 G90 G94 G91.1 G40 G49 G17
N15 G21
N20 G28 G91 Z0. Problem line change it to G0Z16. or a larger number to clear everything that when it moves to the X Y start position it can not hit anything with the tool
N25 G90

(BORE1)
N30 M5
N35 T1 M6
N40 S25000 M3
N45 G54
N50 G0 X5.404 Y52.667
N55 G43 Z16. H1

---

Line N20 is where your problem is remove it or just do a G0 Z16. Z30. or what ever number you want for your clearance plane

Quote:

---

Originally Posted by mactec54

Line N20 is where your problem is remove it or just do a G0 Z16. Z30. or what ever number you want for your clearance plane

---

Yep.
I also always change mine to G0 Z30. Which is my safe Z height.

Well went out in garage to test some of the possible fixes, and jogged the mill to somewhere near center of bed and notice it
was making funny noise, and wouldn't you know it, the aluminum flexible coupling on x axis was broke. Looks like now I will
have to wait a week for replacement part to test...bummer

Quote:

---

Originally Posted by kansaswoodrat

Well went out in garage to test some of the possible fixes, and jogged the mill to somewhere near center of bed and notice it
was making funny noise, and wouldn't you know it, the aluminum flexible coupling on x axis was broke. Looks like now I will
have to wait a week for replacement part to test...bummer

---

Bummer. Are those the spring type ones? Been there :rolleyes:
I switched to the plum jaw type a while ago.

yes they were the spring type. 6.35 to 10 mm are the plum type which resemble lovejoy couplings
free of backlash. Wondered about how much expansion and compression the flexible material would
introduce into axis. I may give them a try also, using nema 23 servo motors that normally utilize 5 amps
under normal load, but can surge to 20 amps for 1 second. Pretty sure that would be enough to
do in the aluminum ones. As of now I have only been cutting foam and the white plastic cutting boards
purchased at wallyworld. Have delrin but prefer to wait until I conquer the outstanding issues before
starting on expensive material.

Quote:

---

Originally Posted by kansaswoodrat

yes they were the spring type. 6.35 to 10 mm are the plum type which resemble lovejoy couplings
free of backlash. Wondered about how much expansion and compression the flexible material would
introduce into axis. I may give them a try also, using nema 23 servo motors that normally utilize 5 amps
under normal load, but can surge to 20 amps for 1 second. Pretty sure that would be enough to
do in the aluminum ones. As of now I have only been cutting foam and the white plastic cutting boards
purchased at wallyworld. Have delrin but prefer to wait until I conquer the outstanding issues before
starting on expensive material.

---

It is a common problem for that type of coupling to break they make them in steel and stainless steel also but are still not ideal for zero backlash

This is the type of coupling you want it is called a diaphragm coupling they come in a single diaphragm or double you can find them on Amazon

Quote:

---

Bummer. Are those the spring type ones? Been there

---

Yep. I have one of those aluminium springs on the trophy shelf as well. or better descibed 2ps of 1 of those springs.

- - - Updated - - -

Quote:

---

Bummer. Are those the spring type ones? Been there

---

Yep. I have one of those aluminium springs on the trophy shelf as well. or better descibed 2ps of 1 of those springs.

New flexible couplers have been installed, along with complete cable replacement due to splices in middle of old ones and
sheath grounded on both ends(motors and controller box). New ones sheaths are only grounded on controller box end to
hopefully eliminate any EMI from power and control cables running side by side in cable trough. With changing the G54
to G56 and adding a G0Z5 below that mill is performing very well on fusion 360 gcode. I still feel more comfortable working
with a G56 offset somewhere near middle of table for now. Motor pin connectors were exposed and prone to be struck by
accident without extreme care, so I have designed some guards and will post pics soon of what that looks like. In near
future I am the removing the mdf mill bed and replacing with 1.5 inch delrin plate topped with 1/2 inch aluminum
plate drilled every two inches with 1/4 threaded holes for holddowns. At that point I hope to try some aluminum milling, which
will include either air pressure mister or cutting fluid mister. Thanks for the help in getting me pointed in the correct
direction.
AnthonyAttachment 442772

Quote:

---

Originally Posted by kansaswoodrat

New flexible couplers have been installed, along with complete cable replacement due to splices in middle of old ones and
sheath grounded on both ends(motors and controller box). New ones sheaths are only grounded on controller box end to
hopefully eliminate any EMI from power and control cables running side by side in cable trough. With changing the G54
to G56 and adding a G0Z5 below that mill is performing very well on fusion 360 gcode. I still feel more comfortable working
with a G56 offset somewhere near middle of table for now. Motor pin connectors were exposed and prone to be struck by
accident without extreme care, so I have designed some guards and will post pics soon of what that looks like. In near
future I am the removing the mdf mill bed and replacing with 1.5 inch delrin plate topped with 1/2 inch aluminum
plate drilled every two inches with 1/4 threaded holes for holddowns. At that point I hope to try some aluminum milling, which
will include either air pressure mister or cutting fluid mister. Thanks for the help in getting me pointed in the correct
direction.
AnthonyAttachment 442772

---

You can use any offset you want it will not make and difference to how the machine will run, each work offset used is referenced from the home position so G54 G55 G56 G57 G58 Etc all work the same way just use what ever one you want

If you don't home your machine and then Set your work offset ( which a lot of hobby users do ) then you have no reference to your machine home

Here are the Basic's of work offsets

Quote:

---

Originally Posted by kansaswoodrat

New flexible couplers have been installed, along with complete cable replacement due to splices in middle of old ones and
sheath grounded on both ends(motors and controller box). New ones sheaths are only grounded on controller box end to
hopefully eliminate any EMI from power and control cables running side by side in cable trough. With changing the G54
to G56 and adding a G0Z5 below that mill is performing very well on fusion 360 gcode. I still feel more comfortable working
with a G56 offset somewhere near middle of table for now. Motor pin connectors were exposed and prone to be struck by
accident without extreme care, so I have designed some guards and will post pics soon of what that looks like. In near
future I am the removing the mdf mill bed and replacing with 1.5 inch delrin plate topped with 1/2 inch aluminum
plate drilled every two inches with 1/4 threaded holes for holddowns. At that point I hope to try some aluminum milling, which
will include either air pressure mister or cutting fluid mister. Thanks for the help in getting me pointed in the correct
direction.
Anthonyhttps://www.cnczone.com/forums/attac...d=442772&stc=1

---

Don`t know what type of Motion Controller you are using but if it is one of the type that runs off 5 Volts USB then it will be very prone to interference, always best to use an industrial type that runs off 24 Volts, way better.
I see you have sheathed your cables which is good but the best way to cut down/eliminate interference is to use the "twisted pair" system for cabling, especially for signal wiring going from your Motion Controller to the Motor Drives, a good example is an Ethernet cable, if you have any old ones lying about they are excellent for getting your "step-direction" signals to your drives.

The G56 has nothing to do with the machines Home position, it is, as has already been shown (mactec54) simply a distance that is a reference from your machine Home position, so here is an example, jog your machine in the X and Y to say the lower left corner of you machines travels and your Z axis to it`s highest point and now set your Machine Zero at that point in Mach3, to make sure it is working correctly now jog your machine away from that position in all three axis, doesn`t have to be far, and then click the "Ref All Home" button, your machine should now run back to the original position, do it a few times to be sure, the machine should return to that position every time, your machine is now "Homed" and should not need changing again so set all your DROs to Zero. Now set your soft limits to the values you originally jogged to. If you have proper Limit Switches on you machine then you can of course Home to them, if not go as above.
Now, to get your G56 for example place your vise/piece of stock (if using clamps) on the bed and using the "Offsets" tab in Mach3 first select the "Active Work Offset" you wish to use in this case G56, now using all the probing system on that screen set your G56 to say the Lower Left corner and top surface of the stock. Go to your "Fixtures" area in Mach3 and check that the X,Y and Z values for your probing are showing in your G56 offset in the table.
When that is done on the same screen do your tool offsets so all your tool lengths are stored in your tool library and go double check them also.
You should be good to go now, the tool offsets and the G56 Work Offset are stored so even if you turn Mach3 off they are remembered, so if you want to do a different job at at different position on your table you would only need to do the X,Y and Z probe for say G57.
Using the Homing system gives you proper repeatability and much easier setting up from then on as every time you turn the machine on you only need to press the "Ref All Home" button and the machine will run to it`s Home position ready to start work straight away :D :D :D
One small tip, if you are looking to machine metals then make sure that your tool are really tight in the spindle as they can be easily pulled out of collet chucks !!

Hope that is of some help to you :D
Regards
Rob

My wood cutting cnc machine uses a hardware store router. I think of the tool length as unrepeatable when changing tools. or at least I've never bothered trying to make the tool stick out the same distance every time.
I work without tool length offsets, just work piece (G5x) offsets xyz. No G43 and no tool table. Each tool gets it's own program and each tool change requires a touch off to update of G5x Z.
It's not a sophisticated method but it's brain-dead simple and reliable.

Quote:

---

Originally Posted by cyclestart

My wood cutting cnc machine uses a hardware store router. I think of the tool length as unrepeatable when changing tools. or at least I've never bothered trying to make the tool stick out the same distance every time.
I work without tool length offsets, just work piece (G5x) offsets xyz. No G43 and no tool table. Each tool gets it's own program and each tool change requires a touch off to update of G5x Z.
It's not a sophisticated method but it's brain-dead simple and reliable.

---

If someone is learning then they should do it to a normal G-Code format, then it will match there cam software, if they ever need or decide to take a job in a machine shop they are ahead of the game and will fit right in