X5 lathe workshift?

[Joeski]

Hello,

I have been programming Hardinge Conquest lathe's for about 10 years manually and now I am using Mastercam X5.I am having a problem with the workshift.In the program it has all my workshift's to 0,G10 P0 Z0.What I do not understand is how Mastercam tells the machine where my Z 0 is.The tool stop feeds to Z0 and seems to be out the right distance but I am confused, where it is getting the information on this.How does it know or did I just get lucky.Any information on this would be greatly appreciated.

 

Thank you for your Time

 

Joe S.

[kh012]

when you prg. in mastercam your tool paths are from the x0/z0 of the part not the machine.

it doesn't know the distance from your machine home to the part z0.

because your tool offsets will be different.

the way that i do it is post out the prg. with the g10's at 0.

then when you set up the machine

you find your work shift value with a qualified tool. then manually edit in that value into the prg.

unless you know the exact distance from the home to z0 on the part ahead of time. this is the easiest way.

 

HTH Ken

[Joeski]

Hello Ken,

I did that and set my P0 X0 Z-1.5 and I have a stop in the machine with good goemetery offsets and it feed out 4 inches,Usally I can rely on my stop as a place to start and touch off everything from there but it does not seem right.I would think with everything at zero the stop should come up to the face of the collet but that's not what happened.Seems weird and what wil happen if I do the job again in a differant machine? I don't get it.

 

Thanx for your time Ken

 

Joe

[kh012]

when you quailfied your tools are you using a probe or presetter or

are manually finding z0 on the part, because with the probe your offsets will

usually be from the turret face or c/l of the turret and be small #'s.

if your qualifing from say the home pos. then you offsets will usually be large #'s.

if you are qualifing each tool from the home pos. then you don't need to use a work shift

because your offsets are basicly your work shift for each tool.

using a probe everthing is qualfied to the turret then you use the work shift to locate the z0

in the machine.

 

HTH Ken

[Joeski]

Well my geometry offsets are done manually,they are the distance that are off the turret,the face and the sides.I do not have a tool probe on my Lathes,just my mills.These numbers are small like 2.5 in X and .995 in Z.Is it that mastercam programs off of the home position? But with everything set to zero it confuses me.Is Could there be something in the post? THANX

[kh012]

ok with the way you are touching off then you need the work shift.

looking at your pre. post you put in a value of z-1.5. this should have

put the stop at z0 on the part or 1.5 from the face of the spindle if the offset was active

when you ran it.

take a look at the prg to see that it did indeed go to z0 stop then open the collet,

feed the bar then close the collet. before going home.

if it does't do this in the prg. then the tool path in mastercam is wrong.

and you are getting a different z value friom somewhere.

 

Ken

[generaldisarray]

I am not sure if I am making total sense of this but here it goes.

Mcam is outputting a parameter write (G10) to set your work shift to zero.

What do you want it to say? Some other value?

 

As for your tool setting, Im not sure what you have going on there. But if it works for you then fine.

 

The industry standard as I know it is the face of the part is Z0. Not always but lets keep it simple.

 

This is accomplished a variety of ways.

 

On an older machine like a Conquest I set the tool Z by physically touching the stock. And entering that z position into the tool geometry table. Minus some for cleaning up the face.

 

Subsequent tools are then "touched off" on the finished z face and set.

 

X values are touched to the stock so that they cut a diameter, Position entered and on the Conquest the resulting diameter is subtracted from the x geometry table . Od or ID dont matter.

 

The only time I use the Work shift is to make multiple parts out of one piece of material.Z should be set to zero before setting tools, unless you are good at math.

 

And X should never be used.

[Joeski]

Yes it did go to Z0 as I watched my position screen.And this is what is bothering me is,where is it getting like 2.5" in the reflection of the differance in position screen.(relative&absolute) The next tool came up to Z zero also,It seems to work but WHERE is it getting this Z value from??I looked in my control thru all the work shift values and they are all zero.

 

Joe

[kh012]

^^^^ this is how we do most of are lathes. but we have quest851 msy.

that uses a work shift for both spindles.

i have the post put in G10 P0 Z[#501] for the main spindle

and G10 P0 Z[#502+#500] on the sub. i do this for each tool.

then at the start of the program it puts in

#501=Z?

#502=Z?

i fill in those Z values when i find the work shifts

it loads those values into the variable page then calls it up as needed.

#500 is used to do a globle offset on the sub if needed for thermal expansion etc.

 

Ken

[Joeski]

As for getting my offset in the past I would add like .500 to the length of the part then put this in the like G10P0Z-1.5 for the main spindle.Bring up the stop and touch off my tools to the face and side of the part.My sub spindle is P0-Z14.875 or so depending on the part.There are no variables set in the program that I can see.Maybe I have been doing it wrong IDK.. I thank you guys for your time!!!

 

Joe

[kh012]

the varibles are something i added so that you only have to enter it once at the

start of the program. not at every tool.

 

Ken

[3rdstring]

I use Miscellaneous Reals (MRs) to output the desire G10 line in the post, I leave it a little long & can then adust it closer to the spindle on the machine.

 

 

pbld, n$, 035, "501", 061, *mr2$, scomm_str, "LENGTH", scomm_end, e$
pbld, n$, 035, "502", 061, *mr3$, scomm_str, "CLEARANCE", scomm_end, e$
pbld, n$, "G10P0Z-", 091, 035, "501", 043, 035, "502", 093, e$

 

#501=1.51(LENGTH)
#502=.35(CLEARANCE)
G10P0Z-[#501+#502]

 

Note: you have to format the variables to output

 

fmt	 11  mr2$	    #Turn Length Macro No 501 - from first op  CJH
fmt	 11  mr3$	    #Clearance Macro No 502 - from first op  CJH

[Joeski]

Good Morning Chuck,

What library is that tool stop in? And Do I have access to that on a level 1 for mastercam? I found the variales page and my G10

location is set to zero.I do not understand where my machine is getting the Z zero location.

 

Thanx

[3rdstring]

The stop is just a modified drill. I have to tell MC the offset for length, #501,mr1.I had to modify the post for the desired output. You have to look at the post & find where the -G10 line is being output.

[Joeski]

Thank you for all your help!!

[kh012]

Yes it did go to Z0 as I watched my position screen.And this is what is bothering me is,where is it getting like 2.5" in the reflection of the differance in position screen.(relative&absolute) The next tool came up to Z zero also,It seems to work but WHERE is it getting this Z value from??I looked in my control thru all the work shift values and they are all zero.

 

Joe

 

you said your tool offset was around .995 and your work shift was 1.5 added up = around 2.5.

the absolute page will read the posisition #'s as they come from the program.

the relative page #'s don't refleck this because it doesn't take into count the offsets or work shift

one way to make them match is actvate the offset in mdi "T0101" look at the position page

and preset the relative to match the absolute.

i usually ignor the reative #'s unless i'm using them to bore a collet etc.

 

Ken