horizontal programming questions

[Ol Slow Hands]

I'm new to horizontal programming, but have plenty of vertical experience.

The parts we mfg are precison XYZ tables, which are driven by leadscrews. So each table typically has four sides machined, with many similar features on each side. The work pieces are typically 12" square or smaller. production volumes are low, typically between 1-25 pcs.

The machining center is a Kitamura H250.This machine has a "on deck" tool changer, so the next tool is always in the changer. The machine is always sent to "home" position when either indexing or tool changing.

Rapid Feed is 1400 IPM

Chip to chip tool change is 3.0

Index is about the same.

The previous programmer typically programmed horizontal parts using the following method-

Machine a feature, such as drill a 1/4" dia hole, index table to the next side , repeat the same tool operation, index again , and so on. When this has been done to all four sides, if necessary, then they change to the next tool. Result = Less tool changes, but lots of table indexes.

My gut feeling is to completly machine one side and then index to the next side, complete that side , index... and so on. Result = more tool cahnges, but less table indexes.

I base this on the premise that since dims are related to each other, they should be machined at the same time if possible.

Which method is the preferred method among you experienced horizontal pros?

 

Thansk for your advise and imput!

John

------------------

 

[Guest CNC Apps Guy 1]

I tend to favor as few tool changes as possible. Doing as much work as possible with no regard to the number of indexes. Indexes are quicker than tool changes for the most part anyway even with rapid rates approaching and in some cases surpassing the 3000 IPM realm.

Mastercam's MPFAN will stage your tools for you so you do not need to add this to the post. Just set stage_tools to 1 and you're off and running.

JMHO

Here's some Topics in the past that have covered Horizontal Machining. You may find these useful:

http://www.emastercam.com/ubb/Forum1/HTML/000558.html

http://www.emastercam.com/ubb/Forum1/HTML/000929.html

http://www.emastercam.com/ubb/Forum1/HTML/000786.html

That shoudl give you a pretty wide variety of how different people do things. In one of threads there is a link to a tombstome that illustrates how I do things.

------------------

James M.

[This message has been edited by James Meyette (edited 05-31-2001).]

[Jcastle]

I agree with James. I also favor as few tool changes as possible. Download the MPMaster Post from the emastercam.com Web Site. it has a bit more options than the mpfan post. Good Luck

------------------

 

[Michael Reynolds]

Is there an advantage to using mpmaster post over the multiple work offset post? I just use that one, and when indexing the b axis, just use g55, g56, g57, etc. Is there a way to use one work offset on all 4 sides?

Mabye it's a dumb question...

Thanks!

Mike R.

[Allan Brown]

The suprep post is a quick way to program for a specific application scenario. V8 toolpath Transform and a V8 post like Mpfan or Mpmaster can be used to replicate the functionality of mpsubrep, while supporting all other subprogram capability in V8.

If your G54 is set at the centre of your rotary axis, you can program using only one WCS value.

[Guest CNC Apps Guy 1]

What Dave said and I'll add (AGAIN) that what programming rotary stuff, you'll save yourself many headaches if you program to the center of rotation, and draw everything how it will sit in the machine. It may cost you a bit of time up front, but well worth it on the back end.

 

Just my 2¢

 

------------------

James M.

[Jcastle]

I have found that programming to the center of rotation is the best bet for most pieces. It does cost you more up front time in planning and documentation. Unlike Verticals the key to Horizontals lays in the Tooling, Fixturing, and Programming The type of work will dictate how you chose to do it. I have also found that it is best to give each face, or rotation a new work plane. Fixtures are never where you think they should be on the pallet. There are many ways to skin the cat, this has worked well for myself.

[Ol Slow Hands]

Thanks for all your inputand advise!

------------------

 

[Michael Reynolds]

Ok, so I'm thick. I accept that...So is what you're saying - set G55 (Fanuc OM) at the center of rotation, then use a template that represents the tombstone, and draw your part on the faces of the tombstone, using t & cplanes? That makes sense, but usually, we put the wcs (G55) on a corner of the part. If I'm understanding this right, then if the WCS is set to the center of rotation, and your X, Y & Z's would look wacked. Also, if you set G54 as the center of rotaion (G54 for me has to be set at machine home) and then had a G0 G91 G28 X0 Y0 Z0, the machine would crash into the tombstone.

What am I missing? Is there a file somewhere that I could look at?

Thanks again, all!!!!

Mike R.

[Guest CNC Apps Guy 1]

Michael,

In one of those topics I referenced above, there is a link to download an example of how I do it. I think it's the middle one or the bottom one.

------------------

James M.

[Toby]

Another thing to keep in mind is if you had cetain tolerances to hold (flatness, perpindicularity, etc) and finished one side prior to rotation some features could move when the other sides are roughed out. It is generally better to rough all sides then finish.

------------------

Toby Baughman

Programming Supervisor

Saint Gobain Semicon Group Inc.

Vs8.1.1 LvL3 Mill + solids