Wait codes again for Mill/Turn.

[crazy^millman]

Ok folks round 27 here on the wait codes. I can do pinch turning inside of Mastercam post the code and get wait codes at every point I want using the cantext method I figured out. Now the problem is they want more. I am now being ask to have it change tools while finishing one operation and have the next ready or even running a finish tool from the lower turret to the last pass on the upper turret roughing after already running 2 turrets when roughing the part. Getting pretty tricky to keep up with depths of cuts so that upper will take say 4 passes, lower will take 3 passes balanced to each others yet the upper will leave enough stock for the finish pass and the finish pass can then start .05 behind the upper turret just like the roughing pass did. Approach at .05 on the upper and .1 on the lower is my best approach here. Ok so now to the heart of the problem. My method work great when doing one upper and one lower tool when pinch turning. Now I need the upper turret wait codes to quit being synced with the tool it was synced with and now wait for the lower turret to get to a place when it can catch up to that upper turret point and now go back to these new operations being synced again. I am thinking I need to know not only use cantext, but need to involve a buffer of some sorts. I need to have the ability to turn off my mi10 variable with is saving the pcode to then increment my wait code as if I were not using the mi10 variable for the 1st operation, but was using all the way through the 2nd operation now for the 3rd operation not use the mi10 for part of it and then start using it again.

 

Here are my thoughts so far. I have cantext 20 as my synced method doe my wait codes so if I were to create say cantext 19 with the unsaving method of my wait codes will the post go between operations and count up on operation 3 when posting, stay put in operation one when posting keep synced with operation 2 and then when I go back to operation 3 and use the cantext 20 it picks back up from where operation one was and then outputs all my codes like I have been doing this time now by hand and through ym memeory method in my head?????

 

Other thought involves finnally learning buffers and then taking the whole posted code putting it to a buffer using a couple switches or cantext as place keepers of where and how I want my code to be and then when I pull it our of the buffer at the end as the complete program then un buffering of the program controls my synced and non synced parts and then posts them all out just like it should???

 

3rd option get Espirit and be done with Mastercam when it comes to doing this type of work????

[MultiAxGod]

quote:

---

3rd option get Espirit and be done with Mastercam when it comes to doing this type of work????

---

 

Gotta love this one! I hate Esprit ! I HATE IT, I HATE IT! I HATE IT! ROFL huh Hardmill? LMAO

Forget everything you ever knew about programming before you even try to use it or you will fry your brain trying to figure out why you can't get a toolpath correct!

They do make pretty pictures of the machine!

It's a tough choice, keep struggling with Mcam or learn a new package that can do the job.

Yes, it does work correctly and much better than Mcam for Multi-Spindle, Multi-Turret machines.

What machine do you have?

 

Just a simple man with a simple plan!

 

Mcam X2-MR2-SP1

Mill Level 3

Lathe Level 1

Solids

5 Axis

[tryon]

Ron,

 

What you have been able to accomplish with mastercam and the wait codes is very remarkable and impressive. What you are wanting this time is the next step and i can see it as being a very tall order. If anyone can do it you can but without simulation before running in the machine i just cant see being able to safley do it in mastercam without simulating everything. What you have now works because its still primarily 1 tool at a time and your are syncing the beginning and and end of each operation.

 

The next step as you said is being able to figure out which tool will get done first and get ready for the next operation and figure out where the upper turret will be when the lower turret is in position ready to cut or vice versa. I dont think mastercam has enough machine parameters in the machine def to actually calculate accel/decel, home position for each turret, index time, etc. for it to know where the tools are at all times. This is were they are extremely lacking. well its lacking completely in syncing but...

I am not so sure if even esprit can get you perfectly optimized yet either(been awhile since i looked into again).

 

My multi turret/spindle expierience is with Nakamura NTY3's. These have 2 upper dedicated turrets and a lower turret that can work on either spindle. For awhile i could imagine that i could get close with mastercam. What i have found out is that it sort of gets me in the zip code. I need a program for each turret. i program for the left spindle and then the right spindle. After that i pull out tools and put them into the lower turret program for each side. Then i add in the proper Codes for which turret is controlling the spindle at any given time. This gets me closer. Then the actual prove out is when you start finding out what your actual timing situation is. And dont forget that if you are proving out a program with the rapids at 25% you will have a completly different timing then at 100%. Makes it pretty scary to proveout. If you want to optimize your program further you will be copying and pasting waitcodes left and right. Moving spindle speed codes up and down and all kinds of things. Then, then when you finaly get to see everything run together you see more subtle or not so subtle changes you can make again. which starts the entire process over again. Depends on how much cycletime you want to save. We run mainly production so its every possible second counts. Its not uncommon when setting up to find that if i took a tool off the upper turret and put in the lower turret that i could save 3 seconds. Then that move opens up other small improvements. Most of them would be easy improvements on a single turret machine.

 

Besides during a transfer i dont use many waitcodes at all. I just counted in one of my programs that has 24 tools total and 140 second cycletime. 7 tools from the lower turret work on the left spindle(4 of them are syncd with the upper turret cutting also), and 3 lower turret tools cut on the right spindle(1 sync'd with the upper turret). i have only 10 wait codes between all the turrets. Ive gotton pretty good at it but its still takes a few hours to get it all together once i am at the machine proving out. I watch it run a week later and still see that i could take a few more seconds off but it would take a few hours to do it. Can Mastercam or ANY other cam possible now how tool pressure is going to affect the dimensions of the part? You really dont know till you get in there and try it.

 

In summery;

If mastercam could do it then i would prefer mastercam. Are they going to hit a homerun at thier first at bat?

 

True accurate simulation is the single most important feature to get all you can out of these expensive machines.

 

Is it worth the time it takes to fully optimize a program? Is taking 2 hours to take 10 seconds off

a 5 minute cycle time for 50pcs worth it?

 

Sorry for this post but its hard not to sound like a crazy person talking about multi axis multi turret/spindle machines. :bonk:

 

Good luck everyone,

[cherokeechief79]

what he said is so true.i am so happy to finally be away from esprit.

btw is this machine a nakamura?

 

 

quote:

---

quote:

--------------------------------------------------------------------------------

3rd option get Espirit and be done with Mastercam when it comes to doing this type of work????

--------------------------------------------------------------------------------

 

 

 

Gotta love this one! I hate Esprit ! I HATE IT, I HATE IT! I HATE IT! ROFL huh Hardmill? LMAO

Forget everything you ever knew about programming before you even try to use it or you will fry your brain trying to figure out why you can't get a toolpath correct!

They do make pretty pictures of the machine!

It's a tough choice, keep struggling with Mcam or learn a new package that can do the job.

Yes, it does work correctly and much better than Mcam for Multi-Spindle, Multi-Turret machines.

What machine do you have?

---

[Guest CNC Apps Guy 1]

I feel your pain Ron... I feel your pain... His machine is an Integrex Mark.

 

From what I've heard and read from CNC, I get the sinking feeling it's going to be X3 MR1 before we get anything substantive in the Mill-Turn side... I already have a seat of Esprit, I just have not gone to training yet. I do have posts for the Nakamuras that supposedly does what you're asking and what we've been waiting for...

 

Is it time to pull the trigger on learning Esprit CNC??? I'm a LOOOOOOOOOONNNNNNNGGGGGGGG time supporter of Mastercam but my patience is running out.

[crazy^millman]

Thanks guys the Machine in question is an Okuma LB-15M. I can pretty much make a program for the Integrex with no problems. No way to verify it or see a crash, but that is what a good set-up guy gets paid for. The Okuma I can make it do what ever I want if I get out on the machine and do it, however like you said I do not have the time to spend hours trying to get something to the owners liking and still get my others jobs done. He was convinced I could take a 1.5 dia shaft turn 22" down to .45 using pinch turning and have no problems in 300M. I did 9" and got the chatter monster he then let up. I spent hours trying to get what he wanted to see. Not that I think the 14 seconds I cut per part on 36 parts was worth it, but hey such is life. I am not sure anything will ever be able to take it all into account, but something has got to be better than having to go out on the machine just to get it the way it is suppose to be.

[Mick]

For a long time, I have been hearing about the new Mill Turn stuff. To date, it has been vaporware, and like CNC Apps Guy says, there is a sinking feeling that X3 wont be delivering it, it will more than likely be X3 MR1 (or later).

 

I've also heard that the Mill Turn turn stuff will be a staggered "machine specific" release. Eg, first released for one type/brand, then another machine type, then another etc etc..

 

And I haven't heard what the timespan between machine releases will be...

 

Now, if the Mori Seiki MT/Nt or Okuma Multus are right down the list, I'm going to have some VERY unhappy managers asking questions...

 

C'mon CNC... You really need to up the ante here...

[Greg Williams]

Guys you are not alone.

[Ployd]

My head hurts after reading this thread! Doesn't sound fun.

 

We do 0 production. Everything is custom so we don't ever get a chance to worry about shaving time off the cycle. However, it can be a pain because everything is different. We are always starting from scratch.

[crazy^millman]

Yeah well my head hurts trying to make this reality all the time. I have learned tons and think the world of Mastercam in other areas. It does pay the bills and put food on the table. However when you start having to pull out hair, want to cut off fingers, and want to start throwing computers through windows because is something then something has got to give. MR1 before we see some things mentioned for lathe, I hope that is all that is about. X3 needs to have mill/turn and piece mealing something based on machines is heading down a path I do not recommend.

[Hardmill]

quote:

---

Gotta love this one! I hate Esprit ! I HATE IT, I HATE IT! I HATE IT! ROFL huh Hardmill? LMAO

Forget everything you ever knew about programming before you even try to use it or you will fry your brain trying to figure out why you can't get a toolpath correct!

---

I remember the frustrations

Logical ?? not at all.

 

 

quote:

---

Yes, it does work correctly and much better than Mcam for Multi-Spindle, Multi-Turret machines.

What machine do you have?

---

Does it get the job done, yes.

Handles the mill/turn stuff with ease.

Like MAG says youll fry yer brain gettin there.

 

 

You know he really isnt a god, just dont tell him that though.

 

 

 

PEACE

[MultiAxGod]

quote:

---

You know he really isnt a god, just dont tell him that though.

---

What? Are you sure!?!?! Don't rain on my parade dude! ROFL!

A legend in my own mind!

 

[Dave Ball]

NX went down that per machine path, where you buy a packaged post and model of the machine with all the kinematics, everything is supposed to be ready to go...ROFLMAO I sure hope CNC doesn't go that route.

[crazy^millman]

Well Esprit will be here Wednesday for a Demo. We will see if we become a dual cam shop or not.

 

[Hardmill]

quote:

---

Well Esprit will be here Wednesday for a Demo. We will see if we become a dual cam shop or not.

---

Well I say you do

It really handles the mill/turn stuff.

All you got to do is get over the head bangin to understand

the logic (albeit fuzzy) of how Esprit works.

Meself and MAG both spent many an hour cursing the

software. Only to come in the next day and it flows

with out a problem.

 

 

PEACE

[Mick]

Looking forward to a report on Esprit Ron

[Rick Henrickson The Boeing Co.]

Ron do you have one touch on your okuma?

[crazy^millman]

No Rick machine is a 1997 machine.

[Rick Henrickson The Boeing Co.]

so does it have IGF?

I know there is an aplications engineer from okuma he is in the mid west and he had a post for the LU and LT I am not sure how he got the P codes working but I know he did I will try and dig up his name tonight and maybe he can help you on this issue

[kazmir44]

i'm very interested in this post.

we have an Okuma LR-25 4 axis that we program with a 2 axis post, then manually input the p-codes; a L470M 2-axis mill turn that we post with 2 posts then edit and paste the code together; and a new LU-400M 4-axis mill turn that should be here next month.

 

Is there any way this post can be purchased?

[Rick Henrickson The Boeing Co.]

I doubt it I think he could help you with the post though it has been awhile since I talked to him but I think I can find his info, I have everything in boxes in my garrage from my applications years with Okuma I just have to find it.

 

Maybe he was hand editing but I dont think so I was working with him at a customer and I am pretty sure he just posted and ran it.

[crazy^millman]

No IGF either. I can get wait codes outputted. Problem is keeping them all in line to each other. Came across another problem today. When using 2 tools you can send both tools home at the same time. If you are using one tool for the upper and 2 tools for the lower then the machine has a fit. So not only do I have to figure out the problem above I know need my sync method to not sync when using more than one tool for a lower operation to the upper operation that is using one tool.

 

Thanks for the replies Rick.

[Rick Henrickson The Boeing Co.]

hey ron this is a single spindle 2 turret right no sub spindle?

[crazy^millman]

Yes that is correct.

[Guest CNC Apps Guy 1]

Had to reccommend a customer to Esprit and PartMaker today...

 

Especially since there's nothing on the horizon...