Sh503 Mori Post

[PROG_MAN_DO]

Hey guys,

 

If there is anyone familiar with the M300 macro on the Mori-Seki horizontal you will know what I am after here, even if you're not I am sure someone will be able to help me out. Currently I have set up our post to hard code the M300 at the beginning of the program which looks like this:

 

G90G10L2P0X0Y0Z0B0

G90G10L20P1X Y Z B0.

M300A54.01 B C54.02

 

The B values in the M300 lines must be put in manually, as well as changing the C value which corresponds to the work coordinate system. One of my stupid human tricks is I can be dyslexic and input the wrong rotation. Can someone direct me as to how I might be able to have the B rotation output as well as the C54.02 change according to the corresponding work offset. For example:

 

 

G90G10L2P0X0Y0Z0B0

G90G10L20P1X-12.401Y-11.497Z6.0775B0.

(the x,y,z values in the line above will still need to be put in by the set up person)

M300A54.01B90.C54.02

M300A54.01B85.043C54.03

M300A54.01B274.899C54.04

 

I will check back here periodically for your help.

 

Thanks in advance

 

[Guest CNC Apps Guy 1]

Are you sure that Ellison did not make you a custom Macro that uses M300?

 

I have 4 Mori Horizontals (1 is an SH-503 as well) and none of them use this M-Code. I can't even find it on my manuals. I found up to M201 in the Electrical Diagram Manual.

[PROG_MAN_DO]

Why yes Ellison did make this custom macro and it's a dream come true in my opinion. Does that make a difference to you?

 

[Guest CNC Apps Guy 1]

Well, if there's a problem with the Macro yes it does matter. Brian is one of the best Macro writers on the face of the planet, and I'm sure he can dial it in for your specs.

 

Now, if your question is "How do I get the values output in the G-Code without having to put anything in", then you have to look at using a T/C plane to emulate that rotation then you have a post that supports that. MPMaster will support one rotation output but not two. If you need two then you'll have to go with MPGen5x in Version 9 and you'll have to get it set up to match your machine configuration. Probably going to cost you some bucks from your reseller but well worth the investment IMHO.

 

HTH

[PROG_MAN_DO]

I guess I was unclear, I too have been programming for quite some time and have a fully operational post (except for a little editing as I was referring to) All I want to know is how to modify the post to do what I asked in my first message.

 

I know Brian's abilities are very exceptional and have been in contact with him for many years, there is no problem with the macro, just the post. Can you help me now?

 

Thanks for the lecture/3rd degree.

 

[Guest CNC Apps Guy 1]

Basically from what I gather from your first post, you want an "A" value, "B" Value and a "C" Value. Now, if those values are known beforehand, then you could actually use the "Home Position" field, put your values for A in X, B in Y and C in Z, but, if those values come from a rotation relative to your part, then you will need some serious work on your post because you then need a 6 axis Post. X,Y,Z,A,B,and C. For plan A, you'll need to have a similar line to this

 

n, "M300", *xh, *yh, *zh"

 

This probably is an overly simplistic solution but with the limited inromation you've provided I can't really offer more. I have no idea where these values are/should be derived from, how/if they relate to the part and it's orientation.

 

Just trying to figure out exactly whay you want.

[Jeremiah]

If I am understanding your request correctly, then

 

A = 54.01 always ?

B = whatever rotation(index) is ?

C = A + .01 at every rotation(index)?

 

Is your post currently outputing B ?

 

If you can verify some of this info it would help.

 

My other .02, Have you ever thought about programming from cl of rotation and hard tooling your fixtures ? We have an MH63 and it works quite well without all the macro's. Just a thought.

[PROG_MAN_DO]

Thanks for the replies guys..

 

Here's the deal. Yes I have programmed from centerline for years and if the tooling is not dead on you know the drill of re-posting. With the M300 macro you program to part origins and the macro does all the calculations behind the scenes and you only have to post once for the rest of your life, provided you are a perfect programmer. We do use hard tooling IMHO M300 is the way to go.

 

Here is an explanation of the output.

 

A54.01 refers to extended wcs G54.1 p1 This is the part origin position @ B0 in this case

 

the B value is the rotation set by your tool plane however many they may be.

 

C is the wcs you wish to write to C54.02 writes to G54.1 P2

 

Therefore the M300 A54.01 will be the same at the beginning of every line only the B value and the C value will change according to your rotations.

 

I don't think a 6 axis post is required, a lot of post work I suspect, that's why I'm asking

 

You could learn a lot from a dummy like me.

 

Does that help you guys

[Guest CNC Apps Guy 1]

quote:

---

I don't think a 6 axis post is required, a lot of post work I suspect, that's why I'm asking

---

No, you don't need a 6 axis post. But when I see ABC that's what I'm thinking. Now we're getting somewhere. You've made things pretty much crystal clear.

 

Ok, it's going to take a bit of work but it is doable by an intermediate post guy. Basically for A you need to modify p_wcs so that you get A54 and the "." value gets called when workofs is 6 or greater.

 

To get B you need to call "pcout" and get it's value.

 

To get C you basically need to be looking at the same thing you were looking for to get A.

 

HTH

[Jeremiah]

Russell- sounds easy enough, as James said. Were you able to get it working?

Pardon my ignorance but what does the M300 macro do that is so great ?

[PROG_MAN_DO]

Thanks James I will try it out first chance I get.

 

As far as the benefit of the M300 macro it stops the need for reposting even if the part is not in the same location on a tombstone for instance, at which point you would only need to change your X,Y, and Z values in the initial G10 line at the beginning of the program which the M300 macro uses to calculate the x and y changes for a given rotation and then automatically writes it to the corresponding wcs based on the C value. No input by the operator/set up person is needed. It makes verification easier for multiple op parts since you don't have to move the geo as far via stlxform. In the unlikely event we have to move the fixture to a different location we will use our probe to pick up a new origin.

 

All that being said, if there is a better way and as I said before, I have done extensive centerline programming, I would love to hear about it. I am always open to new ideas.

 

I will keep you posted as to my progress with the post and respond to any other inquiries as soon as I can.

 

Much appreciated

[Reece L Gibson]

I will help you.

E-mail me

[jeff]

James,

Do you know how I can contact this Ellison guy?

I have a complex macro for a Fanuc O-T that needs Albert Einstein to figure out.

I just need a slight modification.

If not him,do you know of anyone else that might be able to help me?

[Reece L Gibson]

Send it on, I might be able to help you.