Programming 4th axis with multiple parts

[NodecoMachine]

Hey Guys,

 

  I think this is my first time posting a new thread here, so I'll give a little intro of myself and where I work.

 

  Intro - My name is Scott,  I work with my Father in a small shop (just me and him).  We have a 1996 VF0 with 4th axis, H.H. Roberts (2-axis lathe), and a retrofit cnc knee mill.  Our work is becoming more and more complex which I enjoy greatly and this forum among others have been invaluable for me to learn from others.

 

  Question - We are getting ready to run a small amount of 304SS pieces in our Haas VF0.  We will mount 2 blanks into the indexer and that is where my confusions come into play.  I've attached a picture of the setup to help you understand my questions.  There will be no simultaneous 4th axis work, just indexing and machining, and also the parts do not have any tight tolerances (+/- .005 everywhere).  

 

1. Our normal practice is to have the centerline of the index to be Y and Z axis 0 with our single piece jobs.  Should This be the same for multiple parts?

 

2.  I'm going to program so that the machine will do all operations with the same tool at the same time as opposed to completely machining 1 part, then machining the other to reduce cycle time.  How should the offsets be? Should there be an offset for each index? or offsets for each part at each index?  For example just 4 different offsets, 1 being at 0 degrees, another at 90 degrees and so on. Or 6 offsets, 1 offset at 0 degrees (one access to 1 piece), 2 offsets at 90 degrees for each piece...?

 

Thank you in advance,

  Scott

 

TC0007 Fixture Assembly.pdf

[NodecoMachine]

Also, you will see in the picture that there are a couple features on each part that are at odd angles.  I figured it would be easiest to ignore them for this discussion.

 

Thanks again

[Guyinthedesert]

There are a few ways to do this, I would leave my Y0 Z0 as the center of rotation. You could program both parts using G54, but it might give you a little more flexibility to program using a subroutine for each tool, and make one part G54 and the other G55.

[djstedman]

For Part 1 of your Question,

 

You definitely want to have the fixture aligned on the center of rotation Y0, Z0. in Mastercam so that Mastercam knows how to rotate your fixture / parts correctly for Backplot / Verify - that said, using WCS you could actually move your program zeroes around if desired in relation to that, for instance you could shift your Z up to the top of the parts if desired to have your program output with Z numbers that relate to the 'part location' as opposed to being related to the 'fixture location'

 

This is what the offsets in the plane manager are about for X Y and Z, they allow you to have Mastercam output NC code in relation to your WCS you have defined rather than having to be tied to the rotary table / fixture center that Mastercam uses for Backplot / Verify.

 

For part 2 of your question,

 

You could program the entire thing with one work offset, but if your fixture has any runout that will show up in the parts, the goal in any setup like this is generally to have no runout, however sometimes there might be some, so having multiple offsets for different sides allows you to compensate for that by getting the correct offset for each side independently.

 

In your case with +/- .005 on everything as you state its probably not a big deal and you could get away with only one work offset, its important to note however, that having one offset for each indexing position allows you to make offsets for each position independent from the rest, in general I feel this is a better method since its often necessary to make offsets as necessary for each indexing position independent from one another, having only one work offset doesn't allow for this.

 

Programing to rotary center also forces you to have your program be completely output in relation to your rotary center position, this makes it hard if not impossible to spot errors in your NC code for positions etc. if you need to debug things later, if you use multiple offsets as described above, you can output code that is in relation to each individual indexed position.

 

The choice is really up to you what suits your needs best, and how much effort you want to put in, but IMO on parts like that its probably worth the effort to define your planes based on position from rotary center and have a work offset for each plane (each indexing position). It takes a very little bit more time to set it up that way, but the end results are more flexible and more readable at the machine for the setup/operator.

[crazy^millman]

Scott, Offsets could be approached a couple different ways. I would approach it with one offsets. Looking at your PDF I see you have made a mandrel to go into your 4th axis and now you have the 2 parts mounted on it. Using the one offset at the place where you think will make it the easiest on you in my humble opinion. Trying to use multiple offsets for a part of this nature would be a lot of extra work not really needed. There are macros that will adjust your offsets for you, but if programmed tooled and set up correctly I think one would be enough. I have had 20 to 40 different parts on a HMC and only use one offset. All of the tooling was made correctly and I verified their exact positions. The programming would be as simple as making one toolpath for each face then making it an incremental Sub Program then you would just need to call it 6 times once you have positioned the tool at each index.

 

You did not mention if you have Mastercam. Do you have Mastercam? If you do what Level do you have? This part could easily be programmed in Mill Level 1. I would estimate about 1 to 2 hours total programming time. 1 to 2 hours for Setup Sheets and tool list.

 

Hopefully that is enough to point you in the right direction. If not post up your Mastercam file and someone will be glad to point you in the right direction. Excellent post and if not said before Welcome to the Unofficial Mastercam but Official Emastercam forum.

[NodecoMachine]

Thank you guys.  Seems like I was way over thinking it.  1 more question, what is the easiest way to use the indexer without getting all kinds of different offsets.  I always end up going through the program just deleting all the offsets that are not G54.  I assume there's a better way?

[Guyinthedesert]

under planes, change the work offset box from -1 to 0

[NodecoMachine]

Sweet thanks everyone, I really appreciate all the help

[Colin Gilchrist]

You can also go into your Planes Manager, and for every Toolplane you are using, you can set the option to use a specific Work Offset in the Planes Manager. This will automatically update any operation that uses that Toolplane. (It is much easier to change the offset for 4 different planes in the Planes manager, than using the "Edit select operations > Edit common parameters method, since you would have to select each group of Ops separately.)