4th axis (y-offset) programming - please help!

[CaptainPlanet]

Hello experts!

 

I have a problem regarding progamming a toolpath with my fourth axis in Mastercam X2.

As Example file I have a 5-sided pyramid; As Machinetype I use the standard Mill default MM. I deleted the B and C axis in the Machine-Definition-Manger and set the A-axis to rotate around the y-axis.

My 4th axis is rotating(parallel) around the y-axis.

Now I want to have the toolpath generated like this: Mill the first side of the pyramid - then turn 4th axis and do next side and so on. O.K. in this case it would be an x-offset milling.

can you please give me some hints how to get this working?

My Mill is controlled by MACH3, by the way...

 

here is the example file: FILE

 

Thank you very much.

 

Regards, Boris

[Guest]

After looking at your part here is what I would do.

 

Your sides are all equal, so you should not have to create any addition tool planes to create rotary motion.

 

Rotate your part so one of the surfaces is parallel to the X axis. Than machine your top surface that has the edge parallel to the X axis.

 

Then using mill toolpath transform you can set it to rotate the tool plane.

 

 

 

 

[Justin Beebe at Folsom Tool]

CaptainPlanet,

 

I am not sure how your mill is set up but in general the A-axis is supposed to rotate about the X-axis. Once you determine if your machine def is set up correctly you will need to leave WCS set to top and create T/C planes for each side of the part you want to machine. It is the T/C planes that will give you the rotation moves in the program. If your mill is set up like a normal mill you should be able to use the mpmaster 4-axis machine def, control def and post. It will give you the correct axis designations and you will not have to delete any axis in the machine def. The more info you supply us with the more help we can give you.

 

Welcome to the forum

[Justin Beebe at Folsom Tool]

John,

 

Your up early this morning. Isn't it unusual to have the A-axis rotate about the Y-axis. Or are there machines set up this way?

[Guest]

It is, he did say he has it set for the A to rotate around the Y, so I was going to wait and see if he had trouble with the address coming out. A instead of B. As long as he changes the address, his A should post out as a B.

 

He also could have swapped out the A xis component foe a VMC B axis in it's place.

 

A couple of different ways to handle it

[Justin Beebe at Folsom Tool]

I thought the machine set up sounded kind of unusual. Also I agree that Transform is much better than T/C planes for this part.

[CaptainPlanet]

Hi guys,

 

John - perfect thank you so much for this hint works out perfect! Posting your Screenshots was brilliant!

This was only a test for creating toolpaths around an axis with the offset move.

The next thing would be to mill something with different sides. I made a new simple test file like a cylinder head for a model engine; FILE

You and Justin mentioned tool planes I think these I have to create here, right?

I found a vid on youtoube to make more clear what i mean;

VIDEO

After 22 sec it is doing what i would like to do; Mill the top side turn about 180deg and mill the other side. o.k. forget the 5th axis in the vid :-) in my case...

I read through the multiaxis tutorial and tried some things, also but all toolpaths, which came out where more than strange...

It would be nice, If you could give me a hint here, also.

 

Justin, you are totally right, the machine def is really not that how it should be but I just played around a little in order to get something what could work for me. I have a portalmill. The y-axis with atached x and z-axis including the spindle is moving over the table. The 4th axis is on the machine table parallel to toe y-axis, as mentioned. So, with the mpmaster 4axis you mean the file from this site mpmaster ?

can you tell me whats the difference between the horizontal and vertical machdef?

I will change the 4th axis in Mach3 to the B-axis that I can just take the mpmaster file...

 

thanks for your help!

 

Bye

 

Boris

[Justin Beebe at Folsom Tool]

CaptianPlanet,

 

I am still having difficulty determining how your machine is set up. There are two standard types of mills. Vertical mills (Z-axis or spindle is vertical) and horizontal mills (Z-axis or spindle is horizontal).

 

On a vertical mill when viewed from the front of the machine:

 

X = Longest axis and moves left and right

Y = Moves front to back

Z = Moves up and down ( vertical spindle)

A = Rotates about the X-axis

 

On a horizontal mill when viewed from the front of the machine:

 

X = Moves left and right

Y = Moves up and down

Z = Moves front to back (horizontal spindle)

B = rotates about the Y-axis

 

The link you have is the correct link to download the mpmaster machine def, control def and post. The difference between the horizontal and vertical machine def is that one is for a vertical mill and one is for a horizontal mill. What you need to do is determine what kind of machine you are dealing with then use the correct machine def. Can you post a link or picture so I can see what type of machine you actaully have. Then I can help you get the correct machine def set up

[CaptainPlanet]

Hi Justin,

 

thank you for your answer!

After you explanation it is definitely a vertical mill with the exception that my rotary axis is parallel to the y-axis.

After the machine is set up correctly, which toolpath is then the right to mill parts like the second file?

 

Thank yo!

 

Bye

 

Boris

[CaptainPlanet]

Hey guys,

 

by the way - milling the 5-sided pyramid works. I tried it this minute! Absolute great!

There was only one strange thing:

After the toolpath of the first side there was an call like G55 with an x,y,z and a value.

then the machine drove to a total different place where it went on with the second side. After that there was the next call with G56 and the same coordinate values except the a because of the additional 72deg. Hm What does G55-G58 mean or why does Mastercam post this command?

I changed all the G55-58 to G0 and it worked out perfect all sides at the same place.

I made myself familiar with the T/C Planes; O.K. but where or when do I nsert the rotation of the axis in order to mill the test2 part and which toolpath do I use here? Multiaxis, 4-Axis,...?

 

Thank you for your patient.

 

Regards, Boris

[Justin Beebe at Folsom Tool]

CaptainPlanet,

 

Now I see how your machine is set up. G54 to G59 are fixture offsets that allow you to set different part zero positions on your machine. For the type of rotary work you are doing you should have Z0 and "in your case" X0 set at the center of rotation. YO "in your case" can be set at a postion of your choice. Probably what is happening is the machine reads G54 on the first cut and is in the correct position then when it rotates the post processor spits out a G55 instead of a G54 and the G55 fixture offset is not set in the correct position. If you change all fixture offsets to G54 you should not have any problems. (You can also set up your Post to lock on the first WCS so it will always output only one fixture offset for example all G54's). For your information the reason the G0 fixed the problem is because G54 is a modal command and will stay in effect until it is overwritten by another fixture offset. So when you changed the G55 and G56 to G0 the machine was only reading G54.

 

To answer your question about the second part. At a quick glance I would say you do not need a rotary axis to machine the part. As long as the slots are wide enough (I didn't check the size)I would locate it just like you have it and use a facing toolpath for the top and contour toolplaths for the slots making sure to use rough and finish passes, depth cuts, and to always climb cut. If you are not starting out with round stock you can also contour the outside profile.

[CaptainPlanet]

Thank you for your detailed information. This helps me a lot to understand a little more, what is going on.

You are right, I do not necessarily need the 4th axis to machine the part but this was just only an example. I initially asked for the rotary offset machining; John did here a great job with the screenshots. All siedes were eqal so I just could do the transform "around the axis" but what if the siedes are not equal?

lets say i want to engrave different letters on each side of the pyramid for example.

I would have to create an own toolpath for each side and let it rotate in between.

Do you understand what I mean?

 

Really thank you for your assistance!

 

Regards, Boris

[Justin Beebe at Folsom Tool]

CaptainPlanet,

 

To machine various sides of a part with a rotary axis mastercam allows you to create tool planes. There are several options for creating tool planes "rotate", "geometry", "solid face" or just selecting the planes that are pre named in mastercam....front, right, left etc. The general idea is to leave WCS set to top and change the tool and construction plane by using one of the methods I mentioned above. To create a new plane use the plane button located on the bottom tool bar. The T/C plane is what will give you the rotation move. So if you are in a situation where you can not use a tranform tool path you will have to create a new T/C plane for each side of the part you want to machine.

[CaptainPlanet]

Hi Justin!

 

It works out as you told me thanks a lot for your help!

 

Best regards,

 

Boris

[Scrump]

This thread was a lot of help in posting code for a 4 axis setup I have although I'm getting some trouble with posting different offsets whenever the toolplane is changed. For instance it starts out with g54 on the first top plate and then g55 on the next rotation, g56 for the next rotation and so on...

 

any way to keep the offset on g54?

 

 

Another thing, when I code the toolpaths individually, it will post g54 regardless of the rotation.

[CJep]

any way to keep the offset on g54?

 

Yes, you could use the MpMaster post that is free to download from the forum. There is a misc value that allows you to lock on to the first work offset.

[crazy^millman]

Or you could set it up correctly in the workoffsets for the operations making them all Zero and be done with it.