4 axis rotary toolpath

[artant.me]

Hello! 

I'm trying to use an "experimental" rotary toolpath:

I have made a simple testing model, aligned it's center to X axis:

Then i made a toolpath:

Which looks totally awesome, I want to get the "parallel path with rotation".

If i simulate it, i see the chuck rotating around the model:

I expect very most of the movement to be in Z (up/down), In A (rotation) and in X (when moving from one row to another), but no movement in Y.

But when I postprocess toolpath to g-code, I get very different from what i expect.

I get these circular movement in Y and Z:

And that's what i get from G-code simulation app (and on a machine):

My actual machine:

X,Y,Z axis, Rotary Axis (A) mounted along X 

It's not a machine that has an option of rotating instrument around model, but rather the stock rotating.

I'm using Mach3 to operate the machine.

Is there a way to make it work the way i expect?

In a "lathe" style with continuous movement?

How do i mill this detail from all sides?

[engineguy]

@artant.me 

Don`t worry, it is just the way the simulation works, your 4 axis will turn continuosly, not the tool 🙂

Code is correct, the circular movement is made up of many small Y, Z and A moves.

Regards

Rob

[artant.me]

But why is there Y movement at all?

[Anonymous · Accepted solution]

@engineguy is correct on subject of tool rotation around model but you have a problem in your setup.

You want to rotate model around its center point as shown in screenshot and you need to select all models to clear yellow warning flag next to your operation.

[artant.me]

Ahhh! Zero point of the stock, right! @Anonymous Maaaan, thanks, you saved me so much time! Now everything makes sense!

One more question then (please). What is the best way to position the machine zero? Because now it is inside the stock.

Do i have to 'zero' it before i mount the material onto machine?

Concerning, the yellow warning, it doesn't really matter, as long as i am machining the whole thing.

Interesting thing though, when i select the bodies, i still get the warning! Perhaps that's because i'm using Rhino to model and import bodies as .STP files. So, perhaps, they are not 'true' bodies from Fusion''s point of view.

[johnswetz1982]

You would have to indicate what the center of your platter is. And while you dont NEED to select the bodies it is best practice to do so and not have any yellow warning errors.

[Anonymous]

---

@artant.me wrote:

Ahhh! Zero point of the stock, right! @Anonymous Maaaan, thanks, you saved me so much time! Now everything makes sense!

One more question then (please). What is the best way to position the machine zero? Because now it is inside the stock.

Do i have to 'zero' it before i mount the material onto machine?

Concerning, the yellow warning, it doesn't really matter, as long as i am machining the whole thing.

Interesting thing though, when i select the bodies, i still get the warning! Perhaps that's because i'm using Rhino to model and import bodies as .STP files. So, perhaps, they are not 'true' bodies from Fusion''s point of view.

---

What you refer to as "machine zero" is something else. Machine zero is point in coordinate system of machine which refers to axis being at home position, registered against limit switch that restrict physical stroke to designated location for each axis.

From that location, each axis has certain stroke limit away from home position, combined stroke of each axis  creates work envelope in which you can machine parts.

When you program part in Fusion you need to designate where program origin will be and you must coordinate that with how you set your stock in the machine.

This is how machine "knows" where in work envelope your part exists when you run program.

You measure position of stock in X and Y distance form machine zero point and set those values in G54 work offset.

Next you set tool heights for each tool and set Z work offset to same position you used in Fusion.

So if your stock is 2 inches thick and you want to finish part at 1.75 thick, you would set Z0 in G54 work offset at .25 below top of the stock.

You set origin in Fusion to model top and set stock offset in setup at .25.

To set Z0 on stock, bring tool in contact with stock, enter that value in G54 Z register by whatever means machine uses that function, then shift it in Z minus by .25.

So now you have XYZ origin that corresponds to one used in Fusion and when you run program all moves are in reference to that origin.

As you run program you can measure any depth from machined top of model and adjust for size if there is an error.

If you set stock top as Z0, your reference point is gone with first cut and your  Z0 is up above the part ..... in the air.

With 4th axis part origin must be center line of model, you are spinning model around its center.

If you are not taking any stock off of model face, set X0 at model face and zero stock offset in Fusion.

If you are taking any stock off of model face, set X0 below stock by same amount you use in Fusion setup as stock offset.

You can find all this in programming manuals if you Google "CNC programming manuals PDF",... download some free stuff.

One other note, if you don't select model in setup, you can select it later in operation description but sometimes you don't have that option and error message comes up "no model selected".

So, while you don't HAVE TO select model in setup, it is best practice to select it and forget it.