Custom 5 axis cnc

[Anonymous]

Hi im about to finish my custom designers 5 axis cnc, the design is similar to pocket nc.

What im wondering is if im using fusion 360 for all the CAM work, what are my options for finding the work piece?

One thought i had was using an electric zero button for the tool and then if i know exactly where the center of the b axis is based on the machines zero it will know where work piece is.

maybe there is some better way, anyone that can help me out?

[daniel_lyall]

What will you be use to control it

[Anonymous]

Hi! Mach3 if you mean the software.

[RandyKopf · Accepted solution]

@Anonymous

I have a Pocket NC so let me explain what I do know... Hopefully your situation will be an improvement on this.

First off the Pocket NC does NOT support TCP. That is Tool Center Point Programming. It support Basic Fixture Offsetting for 3 Axis Machining. 

If requires the programming WCS (Work Coordinate System) sometimes called World Coordinate System to be at the intersection of both the rotary tables.

If you are able to use TCP you should it makes setup and tracking of the tool motion much more accurate.

A screwy thing Pocket NC did was do Table on Table with the "A Axis" limited to -5, +95 degrees. And "B-Axis" has continuous 360+ rotation. The WCS is a point approximately 0.885 above the B Axis Table.

So this forces certain things to occur. In a CAM setup it's important that with respect to however the part is placed in CAM Setup the WCS Origin needs to be modeled as well.

Now I am able to have the part placed anywhere on the Pocket NC working envelope but I must statically model where it is in that envelope with respect to the Rotary intersection. Kind of a pain. My high end CMS allows me to place a part anywhere and have an origin anywhere and it keeps track of all the 5 Axis math.

To get you started thinking about how SETUPs are done on Pocket NC you can check out this link and download the Nuka Cola example. You will see this static WCS being modeled with respect to the Part Position.

https://groups.google.com/forum/#!category-topic/pocket-nc/anfiQrBirvU

In the photo below you can see the WCS is the Rotary intersection and not based on the part.

But the part needs to be modeled in Fusion with respect to this.

But the Tool Path has a different Tool Orientation.

[daniel_lyall]

with Mach3 at the moment you pretty much have to do it like what randy says, there is a kinematic plugin come out very soon that will make life easier. 

How are you homeing the b axis.

In mach3 you can use probing to find the work pieces what would be the G54 

[Anonymous]

Thanks randy for your detailed answer!

So by modeling with respect to the wcs you just need to home your machine to the limit switches and then start it because the machine knows where this point is relative to the zero?

If so, is this handled by the post processor?

My setup will be very similar to the point where a and b axis rotation intersects is a little bit below where the part will be, but I guess I just have to do model a fixture for that.

[RandyKopf]

@Anonymous

Part of your machine definition in Mach 3 should describe the home distance to/from the A/B intersection.

Typically in the post you'll have a START section that is prior to TOOL CHANGE section. in that START Section you can have commands to safely position to home in Z and XY respectively and AB.

And then it's a matter of describing in Fusion where your part origin is with respect to the AB intersection. So on the Pocket NC by default G54 is the center of the two rotaries. And I typically describe how far the Part Origin is shifted I use G55 for that and it is only the difference from G54 to the Part Origin. I use a G10 P2 L2 XYZ statement and that is the shift amount. In Fusion I make sure my part has a reference point that reflects that same distance away.  But in Fusion 360 CAM I only use WCS as it is defined as the intersection.

I know that seems confusion but its not really. The machine is hard coded to use AB intersection. So by using G55 shift it lets me have my part anywhere in the working envelope. And all I have to do is make sure my part in fusion is positioned the same way.

🙂

[Anonymous]

Okay so i have some questions on this.

I have tried some different stuff today but im not quite there yet.

One thing i'm wondering is, on a regular 3 axis mill Z0 is on the table and
positive movement will move it up.

Should it be the same on a machine similar to pocket NC? (with the z axis
horisontal instead of vertical of course)

And regarding the workspace as i understand it i need to be able to move to
a location where the machine can know where everything is, my first thought
is using endstops.

And the first thought is the endstops i tried have a little arm that gets
pressed, which doesnt seem that exact, is that the best option?

And also something i find a little hard is that with a 5 axis a machine one
position can be safe from collision but if i then move the a axis for
example its not, how is that handled?

You also mentioned that the location from zero to the a/b intersection
should be set in mach, do you know where?
And should i find it by jogging from the zero point?


And a separate question, my b axis is continous, how should i "zero" that
axis?

[daniel_lyall]

@Anonymous use home switches, in Mach3 when you hit home that is all it will do.

if you have the switches defined as home switches when you are just moving the machine around they will have no effect at all.

So you can put a switch, hall effect switch, proximity, inductive switch whatever you like on the B axis when you home the machine it will just do that then when you move the B axis if it goes past the home switch nothing will happen.

so for your A and b just have a home switch, your X, Y and Z you can have home and limit switches all in one.

you B axis I would use a hall effect switch, they use a magnet to activate the switch

[Anonymous]

Great suggestions thank you!

[RandyKopf]

@Anonymous

First off you should design your machine based off the Cartesian Coordinate System and Right hand rule.

https://en.wikipedia.org/wiki/Right-hand_rule

I would spend some time studying that wiki site.

With that said don't be fooled by the looks of the Pocket NC. It is not a horizontal. It entirely based on Right Hand rule. It just happens to be laid on its side for stability and footprint. But the math is entirely like a vertical with rotary tables. So it's Z+ Axis is up away from the part along the spindle.

You can use stops and set values to base part position off a know position. But typically that is done through standard probe or edge finding a corner of a part. it can also be done by moving the side of a tool bit next to the part and reading the difference in the screen values from home to where the edge of the part is PLUS 1/2 the diameter of the cutter. That is done from X then Y and Z is based on the tip.

Your B axis and all axis will have a homing function. That is inherent in hardware and is part of the tuning with Mach 3.

If you like my input put a KUDO on each reply I made 🙂

THE POCKET NC IS BASED ON RIGHT HAND RULE.

 

[Anonymous]

Yeah i have the axis the same way as that i just was a little inside about positive or negative on z

The z axis is a little hard to see behind the spindle..

any idea on the collision question?

[Anonymous]

You mentioned probing or using a edge finder, should the probing be done while the part is in its original position or do i need to rotate it to A90 for example if that is where the program will do its work?

Im thinking that if im doing 3+2 Jobs that wouldnt make that much difference but if it is continous 5axis i want the easiest way..

To me it sounds great if i can keep track of where the part is based on that the machine and mach knows where home is, is that a bad idea compared to probing or similar?

[RandyKopf]

@Anonymous

Wow that looks like great progress on that machine.

As far as collisions I have a pause button I can hit that suspends all motion. And you get a pretty good idea after jogging you machine and then running it where it starts from and where it should be going. As an example, I do a lot of 3 Axis machining. And it requires the A set to 90. So that is one of the first things that happen. And then it engages the envelope of my part with approach move. If it looks to be in the ball park I let it continue. If not I figure out what I did wrong. When you get into 4 Axis it's also very similar you know the approaches and motions and if it looks ok proceeed. Early on I did nick my table by not realizing there was an impending crash in the works. Since then I've been cautious to learn where the machine typically approaches from and finishes at.

Last when all my programs finish I have the spindle returned to HOME Z and then XY to HOME Z then I move the A and B tables home. And now I cut unattended for hours on end no problem.

And as far as the other question on probe and or using an edge finder. It can be a sequential process. So when I do 3 Axis work I use MDI and move my A and B Table to a fixed rotation equal to how I will later cut the part. Then I move the spindle to X0, Y0 and then jog to my part origin and look at the difference in screen values. I uses those to input the G10 statement to then base my program on.

🙂

[daniel_lyall]

@Anonymous more than likely the machine randy has, has a better planner than what mach3 has, Mach3 does not do simultaneous very well at all, so just be aware the cutting wont be that good if more than 4 axis move at the sametime.

onces the guy is finished doing the kinetics plug in, it should be good as, and it has it's own probing routine so that will make it quite good. 

when I find the post I post it here.

that is a neat looking machine

[Anonymous]

I havent heard that there would be a problem with mach for 5 axis before.

What exactly is the problem with mach and continous?

[Anonymous]

Yeah i already did some 3 axis milling on this machine by fixing the a axis
at 90.

But im just thinking about the case of fixture collision features of fusion
360 and im doing say 5 axis wrapping it would be good to be able to do the
programs so you know it doesnt make any stupid moves, but maybe thats not
possible?

[daniel_lyall]

It's just the continuous motion over so many axis moving at the sametime, 3 axis moving at the sametime is ok the planner is only a 3rd or 4th order planner, it was fine 10 years ago not now Mach4 has the same planner at the moment it's getting a new 1 soon.

all the how and whys are over most people's heads, it's some funky math words 

[Anonymous]

Okay i have made some tests moving them all and havent had a problem, but
maybe the problem is when running programs.

Is there a better alternative to use right now?

[daniel_lyall]

There is a speed and angle change problem with it as well useing Fusion/HSM compensation reduce this problem by a lot.

for me above 900 mm/min with 2.5D - 3D toolpaths this is a problem by useing the compensations, (smoothing and feed compensation) it is not a problem as i can have it set to change speed at certain angles.

your machine is small so you wont be going that fast so it may never be a problem on my little machine I have never had a problem that was not my fault it can do 3D toolpaths all day and not have anything go wrong with the toolpaths it's max is 600 mm/min small very old steppers it's a made in 1998 or 99 emco pcmill 30