4th axis setup question

[DaveR]

So this is not really an MC question, it's more of a basic 4th axis indexer setup question.

 

I'm just starting out with 4 axis at this point and seem to have a grip on how to program basic indexer moves in MC, keeping all of the x and y's lined up, post comes out OK and metacut and MC sims and backplots it OK.

 

My problem is how to set up the machine in terms of part offsets and TLOs.

 

My part is just a 6" X 4 X 4 block with the long axis running with the X axis, and through the rotary axis centerline, and my 4th set up as an A axis on a Fadal VMC running format 2.

 

Now the qs:

 

If in my program I use g54, 55, 56 etc, set at various corners of my part, do I edge find all of those spots and store them as g54, 55 etc? If so where is it (how is it) that I tell my machine where the centerline of my rotary table is? Or do I need to?

 

The TLOs. I have had this explained to me once and I think I understand using the longest tool as a reference in G53, doing TLOs for the first side then touching that reference tool off of all sides and referencing all other tools from it.

 

Is that the way or is there some other that I should be using?

 

Sorry for this basic question, I googled 4th axis setup, indexer setup and every permutation of those as well, bought three CNC books over the past few months, and a video on 4th axis programming in MC. None of those sources have any explaination of actually setting a project up on the machine. If anyone knows of a source please let me know.

[Rick Damiani]

If you are indexing only, locating the various sides by finding the corners of the block, and assigning them different work offsets, and you don't have any A moves in your code, then you don't need to worry about the locaoiton of the axis centerline. This limits you to dealing with each side as a seperate program, and will force you to use (and find) a lot of work offsets, each of which will have different values for X,Y,Z, and A.

 

What I do is locate the program zero on the centerline of the A axis. Then I touch all the tools off to a 1-2-3 block on the table and use a test indicator to find the distance from the 1-2-3 block to the rotation center. Since the rotaiton center and the table are always in the same place, the only thing I need to change or find for a new set-up is the X and A coordinate for the work offset. This allows me two different approaches to the program:

 

- Use one work offset and rotate the tool plane in MasterCAM as needed to cut on different sides.

 

- Use several work offsets, one for each index position. All of these offsets will have the same X,Y, and Z values with A being the only part that changes.

[DaveR]

Thanks for your help.

 

 

So to paraphrase just to make sure I understand you. I can use one work offset , say at the upper left corner of my part. I set that as G54 in MC, touch it off and store the X, Y , and A. Set TLOs to the centerline of the A axis. Rotate the part in MC using Tool planes and leave the work offset set to G54?

[cadcam]

DaveR ,really what you want persay is to lay the A axis in say "X". not for your TLOs correct from center of rotation. so all cuts are Postive.

ay for "Y" center of rotation and "X" can be any were along the part.

 

other wise using another corner as "Y" you will need to use diffrent Work offsets for each rotation as one thought.

[Rick Damiani]

DaveR:

 

Let me try to clear things up a bit.

 

If you use the corner of the stock for your work offset:

 

- You must use a different work offset for each index position

- You must not have any A moves in your code

- You can set your TLOs to the top of the block, but must make adjustments for each work offset.

- You don't need to know where the center of roation is.

- You may use named views/WCS to locate Program Zeros whereever you wish

 

If you use the rotation center of the block (centerline of the A axis)

 

- You only need one work offset - located at the rotaiton center

- Your code will contain A moves

- You cause indexing to occur by rotating the tool plane in MasterCAM about the X axis.

- Your TLOs are set to the centerline of the A axis.

- Look in your MCAM9MILLMC9SAMPLESMULTI AXIS folder for a file named ROATRY 4X.MC9 for an example of how to locate the part and the program zero.

 

 

For multi-axis cutting, you have to locate the part WRT the machene's coordinate system for the angles and such to resolve correctly. Indexing is a special case - you can, if you choose, treat indexing as if it were a collection of fixtures laid out on the table. But that means a lot more time spent in set-up, more opportunity for error, and a lot less flexability in programming.

[DaveR]

OK, I finally got it, that last post there Rick finally rang the bell in my thick skull.

 

Using the A axis centerline seems like the way to go if the work will allow.

 

Thanks all for the replies.

[Harryman]

Use the centerline and end away from chuck face, and you'll be all set for that multiaxis mill/turn you'll be getting in a couple years.

[cadcam]

Dave glad to here you got it.

Looks as thow we were all say the same thing just stating it diffrently every time.

[DaveR]

Between you guys and a machinist I know I have a grip on the concept now. Funny how the same thing can be said so many ways, be understood one way and not the other.

 

 

Harryman, a multi axis mill turn machine is a ways off I think, but it's good to dream.