Sign in to follow this  

Recommended Posts

OK gentlemen, this is a new one on me. And I will preface this by saying just because I have not seen this before doesn't mean it hasn't been done. We have a customer that purchased TCP(G43.4) on their horizontal machining center. So I am asking the 5 axis (4?) pros here if they have encountered this?  Possible? Advisable? Better options? I don't want to touch this one since I have absolutely no experience with this use of TCP. But since it's been thrown in my lap, I guess I will have to pursue this. Can anyone comment on this? I would have had no problem suggesting TWP for this application.

 

Paul

Share this post


Link to post
Share on other sites

TWP should be used them if they got TCP. All they have done is passed the the Full 4 Axis comp back to the Controller for full 4 Axis toolpaths. They get an advantage of not worrying where they setup on the machine within reason and reach of tooling and axis travels and program it for one position and run it anywhere they want to.

Share this post


Link to post
Share on other sites
2 minutes ago, crazy^millman said:

TWP should be used them if they got TCP. All they have done is passed the the Full 4 Axis comp back to the Controller for full 4 Axis toolpaths. They get an advantage of not worrying where they setup on the machine within reason and reach of tooling and axis travels and program it for one position and run it anywhere they want to.

So, what are you saying Ron? Use TWP instead of TCP? That was my thinking. TCP should work but isn't that overkill for an HMC? Thanks Ron.

Share this post


Link to post
Share on other sites

Really going to come down to what they are doing and what they want to do on the machine. Overkill to basic stuff yes, for advanced stuff maybe not.

Share this post


Link to post
Share on other sites

I'd spec both though. TWP for Indexing and TCP for simultaneous cutting.

 

JM2CFWIW

 

:coffee:

Share this post


Link to post
Share on other sites
On 4/3/2021 at 5:25 PM, cncappsjames said:

I'd spec both though. TWP for Indexing and TCP for simultaneous cutting.

 

JM2CFWIW

 

:coffee:

Yeah, that's what they got. We sent them a doc for the parameters to set. Let's see what happens. Thanks for the sample code.

 

Paul

Share this post


Link to post
Share on other sites

I'm with James, I'd be making sure they had enough such that they are not limited in any way.  IMHO, compensating full fourth would be the only real reason one would "need" to do it.  But having TCP and subsequently having TWP, would certainly make the machine far more capable with less effort.  A side benefit is that the programs become more portable from one size machine to another from the same builder or if they have taken the time to breakout machine specific functions into sub routines.  Alternate Rotation offsets and calculation routines become a thing of the past, and now you aren't restricted to running on centerline for full fourth toolpaths.  You can not probe a feature and start cutting in relation it, however it lands on the pallet, so long as mentioned before you don't have a tooling reach, travel, or fixture interference.

I have always wanted full blown TCP/TWP on a horizontal.  Oh the time that could have been saved over the years......

  • Like 1

Share this post


Link to post
Share on other sites
1 hour ago, huskermcdoogle said:

I have always wanted full blown TCP/TWP on a horizontal.  Oh the time that could have been saved over the years......

TCP on an HMC is the ONLY way to fly.

  • Like 1

Share this post


Link to post
Share on other sites
1 hour ago, cncappsjames said:

TCP on an HMC is the ONLY way to fly

Honestly, I think all machines with any combination of rotary axes should have TCP, TWP and a slew of high speed lookahead / smoothing / fairing options at this point.  With the way CAM systems can generate code and with the benefits that combining the technologies together can accomplish, people are leaving lots of time on the table, whether it be in run time, setup time, fixture build time, or just in scrap.  It's pretty amazing that more machines aren't equipped.

  • Like 2

Share this post


Link to post
Share on other sites
10 hours ago, huskermcdoogle said:

  It's pretty amazing that more machines aren't equipped.

Believe me, it's not for a lack of effort. Every HMC machine I try to get those options onto them. Sometimes I succeed and sometimes I fail.

Share this post


Link to post
Share on other sites

I remember back 15 yrs ago in an all Matsuura shop doing a set up. I took over from the night shift guy and he had tons of questions for me when i walked in the door. Why does the part look like this. Why is it scrap. Why cant this machine cut a straight line. and on and on. I looked at the part and right away i asked him if he turned on look ahead in the program. Our post at the time could not insert the look ahead codes in right places and so we had to hand edit the programs to turn it on. It was the old GON and GOF codes. I wished all machines had look ahead and high speed options that were just on all the time automatically. It would be so much easier. But all the high end machines need them.

 

Share this post


Link to post
Share on other sites
5 hours ago, Robert Ouellette said:

...GON and GOF codes. I wished all machines had look ahead and high speed options that were just on all the time automatically. It would be so much easier. But all the high end machines need them.

*HON and *HOF...

FANUC controlled machines do have the ability to turn on AICC automatically. It's done by parameter. It's NOT reccommended to run in that mode on high end machines for a variety of reasons.

Matsuuras (at least in the US) have additional options (NANO Smoothing, Smooth Interpolation, etc...) that cannot be turned on in that manner and are important. I'm fairly certain they are not alone.

Spend the time/money to dial a proper post and do it right. It's worth it.

  • Like 1

Share this post


Link to post
Share on other sites

Gon is the yasnac lookahead.

Hon is for the Siemens and gets converted to g131 for fanuc

Parameter 1604 bit 0 will turn on aicc automatically on fanuc. 

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us