lathe canned cycles

[SBA]

I will try to explain this and see if anyone has been there. The lathe is set to diameter on rough canned cycles so in the cycle:

G85 N100 U0. W0. D.3 F.01

the D.3 is depth of cut diameter, .150 per side par pass. In mastercam when backplot is done it is going radius or .300 per pass per cut. The time given when backploting is incorrect because the two are not the same. Is there a setting or parameter to correct this? Is it post related?

[Brendan P]

I'm not really sure about your question.

In my screen/config/start-exit tab,I have my default construction plane set to +DZ

 

In the ruff step over params. if you put in .150,this should take .150 per side.

But when you backplot it,the numbers you see at the bottom of the screen are giving in diameter.

 

I'm not really sure if this is what you are talking about.

I will be glad to help you further if you need.

[SBA]

Bucket, what you are saying is correct. In the rough canned cycle parameters if I set the value to .30 then the program value is D.30 and in mastercam backplot is .300 per side per pass. However on the machine the D.300 is diameter and thus it goes .150 per side per pass. My question is only to do with the backplot time. The backplot time in mastercam is 1/2 of actual machine time. Is there a parameter or setting just for the backplot to make it read the D.30 as diameter or .150 per side and still post as D.300.

[Brendan P]

SBA,I see what you mean now.

I cannot answer this.

It may be something that can be changed in your post as you mentioned.

 

Sorry.

[chris m]

This is not a Mastercam problem per se; it is a post problem. You have to configure the post to output D.300 when you (correctly) set your cycle to .150 depth

 

C

 

Edit/

 

I don't know what post you're using but prcc_call_end in MPLOKUMA looks like this:

 

xstckcc = xstckcc * dia_mult # Removed lccdirx (cdm)

zstckcc = zstckcc * lccdirz

clearcc = clearcc * lccdirz

depthcc = depthcc * dia_mult # 'D' command as a DIAMETER value

 

 

As you can see they are multiplying Mastercam's depth-of-cut (depthcc) by the diameter multiplier to get the value you want.

 

look for prcc_call_end in your post and add that line where I show it; then try it with your DOC set to .150 in MC

 

C

 

[ 11-13-2003, 12:01 PM: Message edited by: chris m ]

[CR]

HI

 

I belive you need to change your post.

you need to set the dia_mult to 2

(this multiplies your rough step value)

 

search for dia_mult and changed it to 2

 

 

dia_mult : 2 #Multiplier for output on X axis (Neg. switches sign of X)

 

depthcc = depthcc * dia_mult # 'D' command as a DIAMETER value

 

 

hope this help

 

(Just starting to learn MC)

[chris m]

Yet another example of 'ask-a-question, get it answered, say nothing'

 

C

[Brendan P]

quote:

---

Yet another example of 'ask-a-question, get it answered, say nothing'

---

You just havn't got over having to trade the Firebird for that mini-van!

[SBA]

Chris m

Thanks for the reply in fact thanks to all. I will try all when I get to work Monday and respond, sorry I did not respond before but it is the weekend and I did not bring it home. The post is for an Okuma lathe and it is I think modified from the standard Fanuc post.

[chris m]

SBA

 

The new V9.1 MPLOKUMA is a terrific post. What machine do you have? If your post is not heavily modified I would strongly suggest starting with the new MPLOKUMA as the older V8 version was not nearly as good.

 

C

[SBA]

We have an LB45 and LB25 lathe. I made the changes to the post as below. This fixed the backplot time problem. Cycle time now matchs machine and "D" value is correct. Thanks chris m. I wish I understood the post more, I feel I have a fare understanding but some things I cant grasp.

 

I have not tried the new V9.1 post yet but I will some day. The current post is not modified alot but is customized to our likes and is V8. It does not have all the new functions in it as the new post most likley does.

 

final post section after changes:

 

xstckcc = abs(xstckcc * dia_mult)

zstckcc = abs(zstckcc * lccdirz * pl_ax_m0z)

clearcc = clearcc * lccdirz * pl_ax_m0z

depthcc = depthcc * dia_mult

[chris m]

SBA

 

We have many Okuma lathes with different controls so if there is something specific you want let me know and I'll try to work with you to get it. The V9.1 MPLOKUMA is MUCH better than any earlier version. If you want to email me an .mc9 file and an example of what your code wants to look like I can give you an idea of how difficult the switch would be.

 

C