5 axis tool WCS-Tool Plane-Construction Plane

[haroldm9123]

Hello all,

i was trying to find some help with something i have been working with for many years but just had a thought that maybe i have been doing all wrong the entire time. While it has worked it might not have been correct.

So....this is the situation.

When i program a 5 axis part i sometimes have to create a random plane to machine from.  My problem is that if i don't use zero, zero, zero for all of the XYZ values, our Hass machine has problems running this.

For example. In (pic A) the part origin is the front left corner. I want to machine at an angle the back right corner (pic B). Unless i put this at zero,zero,zero (pic C) the Hass will alarm out. 

 

I'm sure 'im doing something wrong, however i was self taught many years ago haha

 

Any and all help would be much appreciated. I look forward to learning something, Thank you!!

[crazy^millman]

Where is the Origin for your programming? That is where TOP/TOP/TOP should be. Then all other plane should share that same point for al the rotations. For what I know the machine is not capable of advanced DWO calculations. If the numbers are not called from the same place then the post would have to map that point and then output it in a way their DWO process can then map back to the Workoffet.  Then the machine does all the heavy lifting to put everything where it needs to be taking the mapped DWO position and runnign the code back to the workoffset position. In G68.2 we normally see X0 Y0 Z0 because a lot the Fanuc based machines don't map this correctly. It forces all programmers to program from one point for 1-1,000,000 rotations if doing 3+2 work. Okuma, Heidenhain and Siemens controls all seems to handle DWO much better than Fanuc in this regard.

[JParis]

1 minute ago, crazy^millman said:

if doing 3+2 work. Okuma, Heidenhain and Siemens controls all seems to handle DWO much better than Fanuc in this regard.

Careful Ron, you'll anger the Fanuc god  :D

JK  :)

[crazy^millman]

7 minutes ago, JParis said:

Careful Ron, you'll anger the Fanuc god  :D

JK  :)

No worries we talk quite regularly and he is fully aware his builder does it much better than the majority of builders using the Fanuc controls.

[haroldm9123]

Hey Guys, thanks for the input!

the origin is currently seen in Pic 1. the front left of the block. once i ZERO all other xyz's from any created planes that will then put those plans at the origin, which means if im using abolute my retracts will be insane. However using incremental it can work but then between toolpaths it wont pull all the way back. the work around has been to just run one set of operations at a time. not a big deal but annoying.  Your explanation sounds more reasonable when explained that way haha

[crazy^millman]

30 minutes ago, haroldm9123 said:

Hey Guys, thanks for the input!

the origin is currently seen in Pic 1. the front left of the block. once i ZERO all other xyz's from any created planes that will then put those plans at the origin, which means if im using abolute my retracts will be insane. However using incremental it can work but then between toolpaths it wont pull all the way back. the work around has been to just run one set of operations at a time. not a big deal but annoying.  Your explanation sounds more reasonable when explained that way haha

Then you need to understand how to link toolpaths if you don't want to send home in Z between indexes. Programming one set of operations at a time is just wrong and you need some advanced Mastercam training. You can reach out to your dealer, but CAMInstructor, Streaming Teacher and a few other interactive teaching sites would be a good choice. All else fails you can reach out to a Consultant and have them teach you. Aaron from Vector MFG is an excellent resource. Not to turn down work, but I have a 12 week backlog right now.

https://vector-mfg.com/

[haroldm9123]

Thank you for the help guys!!! much appreciated :)

[MrFish]

On 6/4/2022 at 1:52 AM, haroldm9123 said:

Hello all,

i was trying to find some help with something i have been working with for many years but just had a thought that maybe i have been doing all wrong the entire time. While it has worked it might not have been correct.

So....this is the situation.

When i program a 5 axis part i sometimes have to create a random plane to machine from.  My problem is that if i don't use zero, zero, zero for all of the XYZ values, our Hass machine has problems running this.

For example. In (pic A) the part origin is the front left corner. I want to machine at an angle the back right corner (pic B). Unless i put this at zero,zero,zero (pic C) the Hass will alarm out. 

 

I'm sure 'im doing something wrong, however i was self taught many years ago haha

 

Any and all help would be much appreciated. I look forward to learning something, Thank you!!

Is your HAAS a UMC five axis ?

if so your post should be outputting G254 For DWO control and this allows you it create the planes where ever you like. You should literally be able to use solid face plane creation and just leave the plane at that origin. This makes programming much easier to understand when looking back and the the cut depth numbers make more sense relative to the plane origin.