5 axis programming

[jerms]

I'm looking for some opinions.
We have a Leadwell V30i 5 axis trunnion with a fanuc Oi-MF control. We do not use TCP/ DWO/ TWP everything is programmed to the center of rotation. Over the past couple of months, it had been crashed and rebuilt. The A and C axis no longer rotate together on center and the y-axis is off .010 at A90. The machine builder said that I can have the error automatically written into the post using a G68.2 tilted work plane. I've reached out to my reseller and just had a post written ($3500.00 mind you) that allows me to manually enter the shift in the machine def parameters. Everything is fine with the post for a workaround and does exactly what you would imagine - it shifts the Y whatever value I've entered. For me personally, I do not like that. I do not want my code to be altered. I want my code to be exactly what it is supposed to be. You should be able to read it and calculate everything based on the tool etc. without having to add/subtract a shift from the error of the machine.  If that was the case why wouldn't I just make any rotation a different work offset and change the value there? 

Is it unreasonable of me to think that the error should be corrected in the parameters of the machine, similar to backlash?  How do other programmers feel about this? 

 

Thanks for reading. I look forward to some responses. 

[Leon82]

Twp and TCP make life easier the control will do those calculations

[mkd]

<trying> getting software to correct for major machine geometry issues is not a road i'd like to go down.

 high-end machines have Kinematic files that contain basic info on pivot points and whatnot. They also have comp tables to fudge the numbers like what your are seeing. These are generally not more the .001" adjustments for backlash.

 You would be far better off  getting the machine geometry corrected mechanically and have the tables handle the small stuff, IMHO.

[jerms]

 

 

 

 

 

 

4

3 minutes ago, mkd said:

<trying> getting software to correct for major machine geometry issues is not a road i'd like to go down.

 high-end machines have Kinematic files that contain basic info on pivot points and whatnot. They also have comp tables to fudge the numbers like what your are seeing. These are generally not more the .001" adjustments for backlash.

 You would be far better off  getting the machine geometry corrected mechanically and have the tables handle the small stuff, IMHO.

Thank you. That is exactly how I feel.

[crazy^millman]

Quote

We have a Leadwell V30i 5 axis trunnion with a fanuc Oi-MF control. We do not use TCP/ DWO/ TWP everything is programmed to the center of rotation.

Well to me there is your biggest problem. Why are you using such primitive methods to program your machine? Why not use the G68.2 and G43.3 on the machine and call it a day. Then you make your Zero where you want on your part touch off the place on the material and your off to the races. The way your currently doing it is the fall of many companies today. We had a customer do the same exact thing your doing and kept beating their heads against the wall. They finally listened after 2 years of fighting all of the same things your fighting and got the G68.2 and G43.4 option installed on their machine. The machine builder came in and set the parameters correctly and they were back to cutting Ti parts within .0002 all day long like they had before they crashed their machine. The post is doing exactly what it should be doing because of the crash, but if you went to G68.2 and G43.4 then you could program it like a 3 axis machine touching off the corner of your material or dead center top of your material and be done. Tear down the setup and move it and set it back up and never care if you hit it prefect to dead center. Think about how much time it takes to set your parts up having them dead on to center of rotation. Do you do the same thing on a 3 Axis machine? No way if you are then your defeating the purpose of even having work offsets on a machine. They are there for a reason so use what you got the way it was meant to be used and your life will be so much easier and your company will be more profitable in the long run in doing so. Pay me know or pay me later is what comes to mind. Sorry not meant to be mean or harsh I am just trying to point you in the right direction. Have a great weekend.

[jerms]

I don't think your mean at all. I agree that it will be much more efficient.  I wish we had been using tcp earlier. Unfortunately it wasn't available to me until now.  I received the new post this afternoon from Postable. 

[crazy^millman]

6 minutes ago, jerms said:

I don't think your mean at all. I agree that it will be much more efficient.  I wish we had been using tcp earlier. Unfortunately it wasn't available to me until now.  I received the new post this afternoon from Postable. 

Awesome to hear and good for you and yes your life will be so much easier. 

[PAnderson]

If this is really a Fanuc Oi-F control then you cannot get TCP(G43.4) as an option. It is not available on that control. 4+1 is the best it can do and G68.2 is available as an option. Actually, it should NOT be an option, it should be standard on any 5 axis configuration. But I agree with all the others about NOT programming from the center of rotation. Old school. OK in it's day but obsolete.

As an aside, how can a company rebuild this machine and not correct everything and leave it with some major mechanical errors? I would not have paid a penny for a "rebuild" of this quality. and then to have them tell you to just fix it in your post? Who does this kind of work?

 

Paul