Need help with fusion360 and mach3 5 axis

[Anonymous]

Hello,

I have a 5 axis cnc machine with all movements on table, just "Z" on the head, who is running on mach3. (HY6040 5 axis)

Can you help me with the good PP and the configuration of softwares?

When i use it in 3 axis it's ok but in 5 axis i have offset on "z" axis and "y" axis, and movement are jerk.

I don't find the solution on this forum yet...

Sorry for my english who is not good

best regards

[johnswetz1982]

I will have to ask why you machine/control does not follow normal naming? XYZ>ABC , If I was describing your machine I would call it an AC machine because A rotates about X and C rotates about Z.

[engineguy]

@johnswetz1982 

John, it is a Chinese machine and this is typical of how they do things, yes, personally I would have the Trunnion "A" axis rotating around the macnines X axis and the rotating table on the Trunnion would be my "C" axis, simple yes ??

Not for the Chinese folks, they like to go XYZ-AB, probably just the way they wire the controls up in the factory, A and B probably sounds more logical than A and C, however this time they have gone for XYZ-BA 🙂 🙂 🙂

If I had the machine I would just swap over the "Step/Direction" inputs to the drives, just plug the rotating table motor connector into the Controls "C" axis output and the tilting Trunnion into the "A" axis output, then it would be easier for me anyway to model and create operations !!

The other odd thing about the OP machine is the limit of +45 degrees one way and -90 degrees the other way, makes getting the operations orientation harder from what I can work out 🙂 🙂

All interesting stuff 🙂

Stay Safe

Regards

Rob

[Anonymous]

I Rob,

I hope you're fine

This morning I reinstall mach3 and test again the last PP.

Like yesterday, the visualisation on mach is good, I can see my test piece, but it don't works...

When I run it, my test piece turn arround the spindle but don't touch it.

if I choose +45-90 for B axis it's because if I select -90+90 the bed can touch the frame of the CNC😬...

I have a configuration to select on mach3 to run with this PP?

In fusion360 I have to choose between : TCP-on-off-axe

and

inverse time-PPM-DPM-DPMPPM-TCP

I don't know what i have to do...

Thank again for your help

[engineguy]

@Anonymous 

Now you need to set your machine up by first setting the Home positions if you have not already done this.

Next you need to set your Part Offset by touching off/probing your piece of stock, this has to match what you have created for your Stock in your Setup in your Fusion Program, I have done a small example file for you to go through and observe the settings. When you draw your Model you must draw it as it will be in the machine, it is much easier if you do this at the beginning, try the attached .nc file, it is correct for the orientation of your 5 axis, so load that into Mach3 and just run it through, it should show correctly in your toolpath window.

Are your Axis correctly enabled and Mapped in Mach3 ??

Look at the A and B moves in the attached .nc file and try using the MDI function in Mach3 to move your Axis to the positions of each operation one at a time so you get an idea of how/where your axis will move, do it well away from you spindle 🙂 🙂

Stay Safe

Regards

Rob

[Anonymous]

Thank you Rob

I test it now!!

[Anonymous]

So

I run your programm and see it in fusion I understand.

ButI have offsets, how change it.

I touch with Z axis to create a zero

I have two touch all sides ? if yes, how save the positions in mach3?

when I use 3 axis i just start from a point on the stock, can I do the same thing?

other question, on your drawing, there is a pivot point in the center of the model, how select a pivot point?

I'm lost a little...😥

[Anonymous]

I think displacements are quitte good, A and B turn and move in the good direction but offset

[Anonymous]

Can you show what I have to do with pictures or others?

[engineguy]

@Anonymous 

So, you are saying that the code file I sent you works OK but it is not doing it in the correct position yes ??

I assume that you have no Limit switches on your Trunnion for the A and B axis homing therefore you must set them manually, for the B axis that swings your Trunnion up and back you will nee to use either an Engineers Level (Bubble type or maybe an Edge Finder that you can use to set the Trunnion to be exactly at the bottom of it`s travel and set that to your B axis Home position, same with the A axis turntable, it must be set so that one edge is exactly at 90 degrees to your Trunnion main body.

Once that is done your control will then know the positions of the A and B axis and move to the correct positions when commanded by the G code.

You will also need to move your XYZ axis to the position that you want them to Home to and then set all 5 positions to 0 in your "Positions" screen, now if you then jog your machine away from that 0 position in all 5 axis you should be able to go to your MDI screen and type in this G0G28G91Z0X0Y0B0A0 all 5 axis on your machine should now return to their Home positions all at the same time, to check each axis seperately do a G0G28G91** the stars being the axis you want to move to its Home position

Not sure how familiar you are with the G code, the G0G28G91 will move a Rapid speed, the G1G28G91 will move at the feed speed set by placing an F** at the end like this G1G28G91F100 (mm/m if using Metric), these are home moves so move in Absolute positioning moves.

Once that is done and all axis are moving correctly the correct distances using MDI commands then it is time to set your Part 0, best to do this and then take the part out again for safety, so whatever piece of material you place on your A axis turntable you would use the same size piece in Fusion and make sure it is in the same orientation as the piece on the machine.

On the example I sent I was careful to draw the model exactly as it would be in the machine, it can be done differently but I find that when using multiaxis machining it is best to keep things as simple as possible:)

Now you can do a Part setup by using your usual Probing of the part to determine it`s XYZ coordinates for the centre of the part so that it matches up with the coordinates set in your Fusion program.

Some work ahead of you 🙂 🙂 🙂

Stay Safe

Regards

Rob

[Anonymous]

Hi Rob,

It's ok for the home "0" position of my axis, for A and B axis, I use a comparator micrometer with a magnetic base.

When I click on the switch "go to home" it's ok for all axis and to controle speed of movements, I have a remote controle.

My problem is: when the bed turn to an other position (90deg for example), origines are different, how the displacements of origins is calculated?

I have to modelise the bed and the rotative plate in fusion?

[engineguy]

@Anonymous 

Excellent, sounds like you are "good to go", Mach3 will do all the calculations for you as long as you keep everything the same.

You only need to model your Part in Fusion as normal and create the Stock in Fusion the same as the piece that you have on your machine, no different than with the 3 axis, all you need to do is set the G54 (or G55 etc) in Mach3 by doing your normal Probing to tell Mach3 the size of the Stock and where it is in the machine just the same as you normaly do, just make sure that it is the same orientation in Fusion.

Stay Safe

Regards

Rob

[Anonymous]

So I have just to find the edges of the stock in Y+Y-X+X- as offsets and select the Z0?

use a start point do the same job no?

An example:

if I use a point on the stock in fusion and start my drill from the same point, normally the toolath is ok no?

or select offsets from the edges of the stock is an obligation to know the placement of the sock after a rotation on A or B?

[Anonymous]

When I use 3 axis it's ok but when I use 4 et 5 axis always big offsets the drill cut next to the stock, it is lost😥

[Anonymous]

I feel my machin configuration in fusion 360 is not good, and my machin configuration in mach3 is not good to...

If mach3 automatically calculed a new position after rotation of my B axis, it is wrong

other question, in the visualisation of mach3, i see the toolpath next to the stock... normally the toolpath must be on the stock on the visualisation no?

[engineguy]

@Anonymous 

You will set Mach3 to know where the Stock is in the machine as you normally do, the calculation for the positions of the operations is done in Fusion which generates the G code to tell your machine where to move to, when Mach3 gets the code it already knows where the stock piece is in relation to the X,Y,Z home positions of your machine.

When you probe a piece of stock and save those positions they are your G54 WCS offset position so Mach3 now knows that the centre of the stock is at say X-200 Y-100, in Fusion drilling a hole in the center the position will be X0,Y0 so Mach3 will move the machine to the Part X0,Y0 by moving the distances set in your G54.

That is all you need to do, it gets more complicated when doing flats at angles with pockets but you just have to always remember to set the Tool Orientation in Fusion correctly to the face(s) you want to machine. 🙂

It will get easier with practice 🙂 🙂

Attached is a small sample Fusion f3d file of some holes drilled in a round piece of material, run the simulation and then go through the settings used in thee Setup and each operation and you will see what needs to be done 🙂

Then you can generate the code and you will see in the code all the A and B moves that will bring the correct side of the stock to position for the Z axis of the machine to be at 90 degrees to each face for drilling, for example, drilling the 3 holes in the top both the A and B axis are at Zero, A0 B0, for the first hole in the center the X any Y axis are at you Part X0 Y0 so it is drilled in the center, the other 2 holes are off center so Mach3 moves them over in the X and Y by the distance needed to be in position, not to a Machine position, from this point on as the program runs the Part Coordinates will no longer be the same as the Machine coordinates, this is correct.

Fusion f3d file, Post Processor used and G code (nc) file also attached.

Enjoy 🙂 🙂 🙂

Stay Safe

Regards

Rob

[engineguy]

@Anonymous 

You do not need to make a "Machine Congiguration" in Fusion, it just confuses things so don`t use it for now untill you are more familiar with what it can do 🙂

If the toolpath showing is not in the correct position then it is not correctly set, see the previous post.

I have run the code in Mach3 here and it runs correctly, double check all your and look in the "Fixtures" area of Mach3 and check the G54 settings stored there.

Stay Safe

Regards

Rob

[Anonymous]

Ok Rob I understand,

On my computer, in mach 3, machins coordinates at 0 and my 0 to start are the same.

reference machine at 0 isn't at the extrimity of movement but in the center of the table, i haven't offsets between the types of coordonnees

Is it normal?

[Anonymous]

In mach3 for me fixture are

g54 x0y0z0a0b0

because i haven't got offsets between the coordinates systems

[engineguy]

@Anonymous 

If that is your "Home" position for all 5 axis then it should work, in the "Fixtures" G54 is the same then Mach3 should just off set the distance in the X and Y as in the G code 🙂

Sounds like you are almost there, one small thing, in your Mach3 "General Configuration" set your Rotational as the image, otherwise it can take the long way round, also if you are using A and B axis "Soft Limits" then enable that here as well

Stay Safe

Regards

Rob

[Anonymous]

Thank Rob

I test it