Temores2790

5 axis_Table-Table_Horizontal (AB axis) Configuration

Recommended Posts

Hi this is my first post in the forum, I already know a little bit of how Machine Definitions control definitions and post works.

My questions are the next with the GenericFanuc5axis post can I make a  starter point to get G code for this machine?

or you guys think I need to talk with one reseller?

the machine is a NMH6300 DCG with Fanuc control, for now, Im just looking work 3+2  

 

 

image.png.b72815d9f62005fd2ecb9636e73ab6ab.pngimage.png.6155a82eb1ec3402f39ccbc8eb1b81dd.png

  

 

 

image.png

Share this post


Link to post
Share on other sites

Yes, the Generic Fanuc 5X Mill Post can be setup for a 5-Axis, Horizontal, Table/Table setup. However, it does require that you know a bit about Post Editing.

The Gen Fan 5X Mill Post does not read the setup from the Machine Definition. It uses Post Variables to configure the Machine Setup and Rotary Setup.

The NCI Data coming out of Mastercam does not contain rotations of any kind. It contains 3+2 data, (Paths, relative to Planes), or Vector Data (Tool Positions in 3D Space, given with XYZUVW Vectors.) To calculate Rotary Angles, the Post (internally in the PSB encrypted section) used both Vector and Matrix Math Functions (including the ATAN2 Function), to map coordinates, and calculate rotary positions.

You'll need to modify the Machine Base Matrix (search for 'matb1$') to be a "horizontal setup".

You'll need to translate/rotate your geometry, to be relative to the System Top View. That is how the part should sit "in 3D space". However, your A/B Zero Tool Plane, would be the Front Tool Plane. You would always program Top/Front/Front for A/B Zero. (Using the Generic Fanuc 5X Mill Post...)

Your Primary would be the B-Axis, and your Secondary would be the A-Axis.

rotaxis1$ : vecz

rotdir1$ : vecx

rotaxis2$ : vecz

rotdir2$ : vecy

 

You'll need to test this, but technically you should only have to flip the sign of the 'direction' variables. (vecx becomes -vecx or vecy becomes -vecy).

With those 4 settings, (and 'm_type' set to '0'), and the Machine Base Matrix setup correctly, you are 90% of the way there.

Set 'primary limit low' and 'primary limit high' (and the 'int' values) to +999999 and -999999. This allows the Primary to wind past +-360.

Set 'secondary low and int values' to -95.

Set 'secondary high and int values' to 30.

matb1$ : 1

matb2$ : 0

matb3$ : 0

matb4$ : 0

matb5$ : 0

matb6$ : 1

matb7$ : 0

matb8$ : -1

matb9$ : 0

 

 

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites

I will say if you want to use all the advanced functions and abilities of the machine talk to your reseller and get a 3rd party post. Yes you can get started, but if your company was smart and got DWO and TCP with the machine then your going to want a modern post to do. The Generic post was written almost 20 years ago and not much has been done to it to improve it since then.

  • Like 1

Share this post


Link to post
Share on other sites

HI 5thAxis, well basically here al the programming is from Center of rotation so the plan is will keep the same method in that way we can use the 5 axis machine like a Horizontal 4th Axis when we need it. I just want to configure the post for 3+2 and CL.

  • Huh? 1

Share this post


Link to post
Share on other sites
10 minutes ago, Temores2790 said:

HI 5thAxis, well basically here al the programming is from Center of rotation so the plan is will keep the same method in that way we can use the 5 axis machine like a Horizontal 4th Axis when we need it. I just want to configure the post for 3+2 and CL.

Leaving a lot of profit and reduction of setup time thinking that way. DWO and TCP are meant to use the internal strength and capabilities of the machine so you don't have to program from the center of rotation. By sticking to that method the setups are locked down and the ability to post and go with any setup is reduced greatly. With DWO and TCP any programmer can program any part like for a 3 axis in the setup and where they want zero and then go from there. Colin has pointed you on the right path and hopefully your company doesn't crash the machine and change the COR and have to re post and redo everything programmed before that point. The other advantage of DWO and TCP programming if that were to happen and they cannot get it back exactly to the COR which 99.99999% of the time they cannot then your not stuck having to change all existing programs to the new COR. Many companies I have dealt with in the last decade all went down the same route your company is headed. Small percentage still do COR and fight that fight every time they have to setup their parts and machine. Majority switched to DWO and COR and are busy, the group doing COR are having a hard time getting work or making profit on the work they are getting. I am just the crazy^millman so take it for what it is worth. :)

  • Like 1

Share this post


Link to post
Share on other sites
8 minutes ago, Temores2790 said:

We have a lot of 4thAxis Horizontal and couples of Integrex Mill-Turns and for all is the same method COR,

 

Good and like I said I am just going by what I see the industry doing to be competitive and productive. The company you work for has figured it out keeping it like it has been for the last 25 year programming these types of machines and not using the options machine builders are providing to make it easier then great. Press on and keep making chips.

Share this post


Link to post
Share on other sites
On 12/9/2019 at 9:08 AM, Temores2790 said:

HI 5thAxis, well basically here al the programming is from Center of rotation so the plan is will keep the same method in that way we can use the 5 axis machine like a Horizontal 4th Axis when we need it. I just want to configure the post for 3+2 and CL.

Smells like "... we've always done it that way..." to me. That is the WORST reason to do something IMHO.  Not a fan of COR programming anymore either. Too many things to fight with when functions exist to make things much more simplified. 

Like G68.2 for example. Which you can get on an HMC BTW. It works pretty awesome too. Easier than G54.2 once set up properly. 

  • Like 1

Share this post


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

Smells like "... we've always done it that way..." to me. That is the WORST reason to do something IMHO.  Not a fan of COR programming anymore either. Too many things to fight with when functions exist to make things much more simplified. 

Like G68.2 for example. Which you can get on an HMC BTW. It works pretty awesome too. Easier than G54.2 once set up properly. 

well is more we've always done it that way, and it has worked quite well in time and the way we want. am not afraid about DWO but I want just start to use MC with the 5axis machine Actually we are using other CAM to program the Mill-Turns and the 5 axis machining when we need it, but that is because we don't have the post correctly for MC to work with the 5 axes so I am taking the first step to achieve it and, so to start to running I need first learn how to walk (talking in the 5 axis post)

am very interesting to have a post with DWO working at all but if I don't have I need to start with the basic post and start to develop as I need 

but thanks for your comments are very helpful 

Share this post


Link to post
Share on other sites
2 hours ago, cncappsjames said:

Smells like "... we've always done it that way..." to me. That is the WORST reason to do something IMHO.  Not a fan of COR programming anymore either. Too many things to fight with when functions exist to make things much more simplified. 

Like G68.2 for example. Which you can get on an HMC BTW. It works pretty awesome too. Easier than G54.2 once set up properly. 

You aware with the Fanuc 31i A5 and above controls on non titling heads that you can run everything in G43.4 and don't need G68.2 anymore on 5 Axis machines? Canned Cycles and everything else is working with no problem on the few machines we have tested this with.  

Trick is getting the post to think it is outputting G68.2 when doing this for the correct Axis mapping, but then not output the G68.2 start and end codes. 

Saving customers money and expanding their capabilities. :)

  • Like 2

Share this post


Link to post
Share on other sites
9 minutes ago, 5th Axis CGI said:

You aware with the Fanuc 31i A5 and above controls on non titling heads that you can run everything in G43.4 and don't need G68.2 anymore on 5 Axis machines? Canned Cycles and everything else is working with no problem on the few machines we have tested this with.  

Trick is getting the post to think it is outputting G68.2 when doing this for the correct Axis mapping, but then not output the G68.2 start and end codes. 

Saving customers money and expanding their capabilities. :)

I just use G68.2 to pre-position then cancel, then activate G43.4. 

From what I understand getting the generic FANUC 5-Axis to post EULER angles can be nerve racking. Thankfully I don't have to worry about such nonsense. 🤣

Share this post


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

I just use G68.2 to pre-position then cancel, then activate G43.4. 

From what I understand getting the generic FANUC 5-Axis to post EULER angles can be nerve racking. Thankfully I don't have to worry about such nonsense. 🤣

Yeah me either working with a Postability Post and were good to go. 

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

So for Okluma osp what are the options? Call oo88 and g169?  I have been using COR but want to go the modern route. How about Okluma 4x?

Share this post


Link to post
Share on other sites
19 hours ago, lowcountrycamo said:

So for Okluma osp what are the options? Call oo88 and g169?  I have been using COR but want to go the modern route. How about Okluma 4x?

I can't say been to many years since I have been on one of their controls to give you a good answer. Brad or Doug would be the better ones to ask. Hopefully they will read this topic and chime in. 

Share this post


Link to post
Share on other sites
On 12/16/2019 at 10:11 AM, lowcountrycamo said:

So for Okluma osp what are the options? Call oo88 and g169?  I have been using COR but want to go the modern route. How about Okluma 4x?

Yes correct or you can use the new G605. For 4 axis there is a also a callOO88 function. If your machine has IMAP it will automatically track B axis indexes

Share this post


Link to post
Share on other sites

Just for the record one can still use DWO while programming COR.  Post edits as such are easy as well.  Even with all of the machine/control goodies I still prefer to program COR.

Having said that, I'm still of the belief that a bought post is worth every penny.  Postability is my first choice.  Be aware you will still need to make customizations and tweaks for preference as well as the occasional hard edit.

  • Thanks 1

Share this post


Link to post
Share on other sites
On 12/22/2019 at 6:02 PM, jlw™ said:

Just for the record one can still use DWO while programming COR.  Post edits as such are easy as well.  Even with all of the machine/control goodies I still prefer to program COR.

Having said that, I'm still of the belief that a bought post is worth every penny.  Postability is my first choice.  Be aware you will still need to make customizations and tweaks for preference as well as the occasional hard edit.

I use to think that way as well until I started using CYCLE800 and TRAORI the correct way with a Siemens control. Now I am convinced the majority of Fanuc builders don't know how to set up the machine correctly to really harness the DWO and TCP. Matsurra does a great job, but it seems other builders are not. The Okuma is just a different control and process so they have a good grasp on TCP and DWO after years of fighting it. 2020 is going to be interesting year and see some major inroad made with the builders to help the industry coming. Really wish my friend Tim was around to lean on, but he passed me the torch so I will do what I can to help as many as I can just like he did. Sorry still not a blogger, Facebook or any of that stuff. Emastercam is my Social outlet so will help as I can going into 2020. 

  • Like 1

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

  • 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