new to mazak

[kendo]

thanks in advance for all the help I'll be asking for in the near future now that I'm a Mazaak-er.

I can look at a mazatrol program and figure out pretty much whats going on, but here's my first problem:

the part is being contoured on 3 sides using lines and arcs, first pass with a 3/8" endmill, then a .02" finish pass with a 1/4" endmill. Theres a line for each tool and the ZFD for both is set to G01.

The 3/8" endmill feeds to cut depth like expected, but the finish tool rapids no matter what I set its ZFD to. I looked through the manuals and found Parameter E17, which is set to 4. When I changed it to 2., the 3/8" endmill fed half as fast, but the 1/4" endmill still went rapid.

I found no other parameters related to this when scanning the books, so I'll be grateful if someone can point me in the right direction on this.

[CNCRim]

Hmmm TPC on rough tool and finish tool is match?

[kendo]

don't know TPC,

Im REAL new to Mazaak

[kendo]

ahh, yes... Tool Path Control, found it

but, it says "No TPC Data Found" when I look for it on both tools

[jimiscnc]

Concepts - TPC means temporary parameter control AND/OR Tool path control.

To create a TPC, display the program, GET INTO The EDITOR, cursor on first line of unit, then menu button (rightmost) gets you to page 2 of edit softkeys. one of them is TPC. This will display a page of TPC info - top half is parameter related. Note you can only change parameters as listed. Bottom of page is Tool path change.

(display button is leftmost - this brings up most pages. menu shows additional pages of active display) (display map s/k is a good one to help the new mazatroller navigate the control)

For example - if using a tailstock then TPC for tool path is reccomended to program turret index position approach to workpiece. and also retract to turret index position.

so, a rough and finish straight turn with tailstock would require FOUR TPC mods - rough tool in, rough tool out, finish tool in, finish tool out.

bad example, looks like you have a milling machine?

THERE IS A MAJOR IMPROVEMENT in mazatrol milling going from Fusion and older to Matrix. Matrix includes many additional capabilities never before seen in mazatrol. Part of that is the Z infeed can take a two place number understood to be percentage of feedrate, for entering the cut. There is also ramp and helix entrance for milling on Matrix. Matrix made this one small item a science.

mazatrol milling was about the same program format from 1983 to 2005. Matrix introduced in 2006 was a sweeping upgrade to mazatrol while also respecting the legacy of mazatrol.

There is the possiblity of seeing a softkey named TPC - this is an additional s/k that merely displays TPCs already set.

In a mazatrol program, there is a white cross and blue rectangle in thte first line of the unit to signify TPC has been applied.

TPC tweaks only apply to the unit they are attached to. Once the unit has been executed, you go back to the global parameter settings.

-jim

[kendo]

Well then , I guess the TPC data for both tools is a match since there is none.
I found the other TPC key, but when I tried it it told me "TPC data creation not possible"

So im still stuck wondering why the rough tool feeds, and the finish tool rapids to cut depth.

[CNCRim]

Kendo,
Try post your question at integrexmachinist.com, they can answer you question most people there are special with Mazak. They should able to help.

[bildoo]

If you do your profiling in one unit (ie. line out) with a rough tool and finish tool with finish allowances. The finish tool will ALWAYS rapid down most of the way to the finish surface then feed the amount of your finish allowance in Z (if no fin Z then it will rapid to depth). The control does this because it assumes there is no material to remove because it removed it with the rough tool before. I am pretty sure there is a parameter to change the amount it leaves for a clearance. I don't think that parameter is available in TPC, only in the parameter page. The way to program around this is to do your line unit with allowances. When the control devolops the rough and finish tool line fill in the rough and then erase the finish tool line. Then program your shape. That unit will only rough the part leaving finish allowance. The next unit you write, do not leave finish allowances. The control will devolop only a rough tool and it will feed the total z depth at the rate set in the ZFD. (G1, G0, or a multiplier) and cut to the programed shape.

I am at home now with no access to a parameter book till I go back to work Satudray morning. I will try to remember to look for the parameter for you. There may be several a bit to turn on or off and a value. Also there is different parameters for 1: Line Left or Right or Center and 2: Line In and Out.

Hope this helps


******UPDATE****

Parameter E95 Bit 4 (1 - rapid to surface + E9, 0 - feed) (E9 is the clearance value) controls this for line machining. It is also available to edit in TPC. The only issue I found is if set to 0 then the machine will feed from Z 0 to cuting surface every roughing pass also. So if you are taking a lot of roughing passes this could add lots of time. If ZFD is set to G0 then it will still rapid in each pass. If you need to change these parameters for other units ie slot or pocket here is the list.

E91 Bit 4 for Endmill Mountain
E92 Bit 4 for Pocket
E93 Bit 4 for Pocket Mountain
E94 Bit 4 for Pocket Valley
E95 Bit 4 for Line Machining (left, right, center, in, and out)
E96 Bit 4 for Slot
E97 Bit 4 for Endmill Top

These parameters apply to both Matrix and Fusion controls and most likely to M-plus and M32 but I did not verify.

[jimiscnc]

damn good mazaking there, bildoo! spot on!

-jim