mori seiki nh4000, fanuc 30iMB and g332 question
Can someone please explain this to me in simple terms. Is this the same as G5.1 Q1 or similar? What is the difference?
Similar Threads:
On my Duravertical, G332 sets the cutting mode. R1. (speed priority) - R4. (better accuracy)
For example:
G332 R1. (SET CUTTING MODE)
G05.1Q1 (ACTIVATE AICC)
I had Mori tune the settings for R1. to get the fastest and smoothest motion while roughing at high feed rates.
I usually use R2. for finishing.
Surprised at how fast and smooth the machine is with AICC. It's only a 0iMC after all.
So you use them together? This is a little confusing to me as it was explained to me that all I would need to use is the G332 and that it "replaces" the G05.1Q1.
I am trying to create a post and am trying to get the correct information before getting too far.
Thanks for the reply!
Yes, they are used together. Once the cutting mode is set you don't have to write it in unless you want to change it again.
So, if for example you wanted to use R3. on all tools, just write in in for the first then you only need G05.1 for the rest. From memory the default is R3. if you don't set a cutting mode yourself.
Have you got manuals for the machine? it should all be there. Still doesn't make much sense initially though......
For my post, I have it writing in G332 R3. every time. I just manually change it to suit roughing or finishing. I guess I could have the post automatically write in the appropriate setting......
I dont have the manuals yet, and in fact I do not even have the machine yet. I am trying to prepare for it.
I have been talking to the applications guy and he gave me a post for the machine but it is mucked up. It doesnt post B axis rotations and it is set up to post for HPCC rather than AICC. We purchased the machine with level 2 AICC (hope that I am not lying here) so the codes that he is telling me will work with our machine I dont think are correct.
I emailed him today and he is still telling me that I use G332 R1-4 in conjunction with G5 P1000, which if I am not mistaken, is HPCC.
I think that one of us are confused.I better make that both of us.
I have managed to create a post that outputs the high speed machining code but i need confirmation.
After what you have said here, the G332 is not used until the High speed machining code is fired? is that correct?
Thanks! You are definitely helping.
Well firstly, remember my machine has the 0i control, so it may be different. I did purchase the AICC option though, but it would be more basic than what is available for the NH.
The manual says that G332 is used to set the cutting mode when using "AI look ahead/AI contour control" So the answer to your question is Yes, G332 is only used once hsm is fired.
Other ways to set the cutting mode are the "cutting mode selection" screen or setting the cutting mode with a MAPPS parameter.
To me, it seems best to always use G332 so you can change the cutting mode to suit the operation you are doing. That works well for me, and the difference is definately noticeable.
My machine doesn't use the G5 P1000, etc. Not sure if that is for HPCC or AI nano or what.
Here's some pics. One showing some code where I have used AICC, and the other showing the "status" notice the "R3." The blank box flashes "AICC" when activated.
Oh, and dont forget the G49 (tool lenght offset cancel) before calling up AICC. If you don't cancel the tool offset it will alarm out.
Then do the AICC stuff, then call up your tool offset as usual.
Ok, a couple of things,
First, here is what our applications guy sent me today. It cleared some things up.
The new 30i series controls (your machine) can accept a number of
commands to activate the look ahead function. The older controls had 4
different look ahead types with at least 3 different command types.
This has bees simplified on the newer controls. There are only two look
ahead options Type I and Type II.
The newer controls will just take the look ahead command you give it and
turn on the which ever function you have.
You have optioned up to type II. You could use either of the other
commands G5 or G5.1 but to take full advantage of the option you have
purchased you will want to command G5 P10000 (on) and G5 P0 (off).
With all that being said there is also a parameter that will essentially
have look ahead on all the time, except when doing tapping. I have not
tried to use this option as of yet. It may be best to build the G5
command into your post.
The G332 is only a Mori function and you will not find it in any Fanuc
information.
Hope this helps.
Brian
Next, Ive been reading about having to use this G49 cancel tool offset prior to recalling the high speed function.
Ive also read that you cannot change the G332 R value until the High speed function has been canceled.
I was curious about a scenario. If you are machining aluminum at very high speeds, and roughing and finishing with the same tool, you could not very well cancel the high speed function and add a g49 in the middle of a single tool cycle without a crash could you?
The reason that I wondered about this, was if you wanted to use a G332 R1. for the roughing, and then to run a finish contour, change to a G332 R3.
I assume that this scenario is not possible?
I always finish with a different tool, so have never tried to change the G332 on the fly. I could write it into a program to see what happens.....
I guess the safest way to change the R value would be to return to Z0 as if you were doing an M6. Cancel and recall AICC with the new R value, along with cancelling and recalling your tool offset as well of course. With the NH it would probably take less than 2 seconds
Hi,Originally Posted by HYPERTUNE
I am curious to know if your control runs windows in the background or not. We have an NH-4000 (2005) MSX 501 and it runs Windows.
Kel1
Yes, it does.
I assume any MAPPS control runs windows to give you the interface, and probably the hard drive DNC functionality.
Still Fanuc running the machine though.
Hello,
I am haapy to you all thru this CNC ZONE .Please keep in touch.
Thanks
Jabu
yea you guys basically nailed it on the head.
what G332 does is give priority to speed or accuracy depening on the R1-4 selection. R1 gives you move jarring accel/decel in corners and such with a speed priority rather than accuracy so you have to be careful when using R1 because you might overshoot your dimensions when you use R3 or R4 for finish cuts (which accel/decel's much slower/smoother).
Re: mori seiki nh4000, fanuc 30iMB and g332 question
Oops, never mind.
It seems there is no way to delete a post.
Re: mori seiki nh4000, fanuc 30iMB and g332 question
Hello i have a question...
i have mori seiki sh403 mill with sh501 control i belive thats fanuc i18
and i have the same problem with h/s cutting
but G332 and G5 dont work on my machine....
G49
G322 R3 alarm come out umber not found
G5, G05.1 inproper G code....
can some one help??
Posting Permissions
Reply with Quote