3 axis programming

[Joels]

Hello,

I am programming a mazak integrex 300S. When i program the sides of the part that are parallel to the standard planes such as front, back etc, the size and depth comes up good.

When i program a 45 degree angle, i set up a plane and it seems the depths do not come up right. i always have to machine the part and then adjust the program. does anyone have a idea what i am doing wrong? od is this just the way it is?

[Guest CNC Apps Guy 1]

You SHOULD be working from one common plane origin. I have a feeling that when you change planes you are changing origins as well.

 

HTH

[Colin Gilchrist]

When programming for a machine like that using only planes, you should have your WCS set to TOP the whole time and you should only be changing your tool and construction planes.

 

James is also correct that all the planes should have the exact same origin.

 

Open your View Manager and click on your "Top" WCS. Look at the numbers in the origin fields.

 

Now press the down arrow key to jump to the next Plane and the numbers shouldn't change...

[Joels]

Thank you for your input. I did as you said and the numbers are changing. I assume i set all the numbers to zero?

[gcode]

quote:

---

Open your View Manager and click on your "Top" WCS. Look at the numbers in the origin fields

---

There is an easier way

Click on Planes at the bottom of the screen.

then Named Views..you will get a chart

will all defined views and origins..

If you are programming from centerline,

you should see nothing but 0's in the origin

field.

[Joels]

I see all 0's but the tool path is still off. the part is square but it has 2 angles of 45 degrees. When i machine the first 45 degree the depth is off. I set all the planes to zero and the tool to zero but the depth is off by atleast .5. Any ideas. Is there a better way to program this part?

[Joels]

i will try to put the file in the FTP site. I will name it joel

[Joels]

it worked the file is in the x3 file folder. can someone take a look and see what i am doing wrong? the planes in question are the pressue guage plane anf the face plane. the pressure gauge plane is about .5 too high and the face plane is about .3 too low when i measure the part on the Mazak.

[cobra95kev]

quote:

---

If you are programming from centerline,

you should see nothing but 0's in the origin

field.

---

That is only if your TOP WCS is at the mastercam original WCS zero point. If not the the numbers will change when you change planes because they always go back to the original WCS zero.

[Joels]

Anybody have any ideas? I am OTC.

[Guest CNC Apps Guy 1]

Take a look at the joel-using correct planes.mcx file.

 

That what you're looking for???

[Joels]

cnc guy. thank you for the reply. I looked at the file and i don't fully understand what is going on but i will try it. I guess i am getting confused with the mill/turn issue.

Thank again

[Guest CNC Apps Guy 1]

Ok, I made the WCS be "LATHE WCS" for ALL of the OPS, then each toolpath has a different T/C Plane. Also, two of the paths had wrong depths in the operations.

[Joels]

i guess i don't understand why i would make a world z for a lathe when i am doing mill work?

[Guest CNC Apps Guy 1]

Because at the end of the day it's a lathe no amout of milling you do will change that. The Axis Orientations are the same as a lathe also.

 

X is Diameter, Y is Off Centerline, Z is paralell with the Spindle, B axis is the head rotating around the Y Axis, and C-Axis is the rotary axis around/of the spindle.

 

HTH

[Joels]

See if i have this right. no more top plane us the lathe z plane. Do not call out a plane unless they are parallel the front, back, etc.

correct?

[crazy^millman]

Joel, I just looked at your program and you programmed it correct, however I see nothing for your misc values. Also need to fix the back view and bottom view since they are the Mastercam default one which are always wrong. I normally just pick the correct one and then make then Back and then Mastercam will ask you if you want to replace I always do. Same thing for the bottom view. Easiest way it ot be in top view. Click in C-planes, Rotate around X -90 deg for Back. Then go back to top View and then rotate around X -180 and then name bottom again it will ask you to replace and now you know you got the correct one. (Yeah pretty weird always has been you can complain, but it will do you no good) What post are you using for this machine? If using the In-House post they have a G68 switch for our type of E-Series and not sure if they are handing that through a G53.5 or still using a G68 on your machine. I would expect to see some values and see nothing, but it could be the way it loaded in my version since you did not .z2g the file. What are your settings like on your mis? Can you post a screen shot of it? Or send me a .z2g of the file? With the post so I can see what is going on.

 

HTH