What is the use of RTCP?

[Shiva.aero]

Hello everyone!

Can somebody please explain what is the use of RTCP for MACHINING?

After a little search, I understood that RTCP simplifies the Post processor calculations by allowing to consider only one vertical tool offset, instead of calculating offset at every inclined angle.

But this seems to be an advantage only to those who write post-processing codes. As for programming is considered, we know that there is no advantage / change for RTCP. 

As person who does only programming and machining, I like to know what advantage the RTCP offers?

Some people says that the RTCP allows us to mount the part arbitrarily instead of exact center of table. But even without RTCP, the program will run from the define part center (G54) & not from the table center right?

Thank you!

[Leon82]

Yes tpc you can probe or indicate the part in, set g54 and go.

With Camplete it doesn'atter how your planes are set. A program for an ac Machine can be reposted for a bc machine with no modifications. You don't even need a new nc format

[GoetzInd]

Allows for the use of normal linier feed rates vs inverse time or DPM. Also allows for smoothing of TCP which limits micro gauging thus improving surface finish and making all around smoother motion. 

MIke 

[Rocketmachinist]

 

[Shiva.aero]

9 hours ago, Rocketmachinist said:

 

Thanks for the link Rocketmachinist!

So in simple terms, in RTCP mode, the WCS or G54 is attached to the Part & move with it, instead of getting fixed to the machine or space.

Is that all or anything more to it?

 

[Shiva.aero]

2 hours ago, Shiva.aero said:

Thanks for the link Rocketmachinist!

So in simple terms, in RTCP mode, the WCS or G54 is attached to the Part & move with it, instead of getting fixed to the machine or space.

Is that all or anything more to it?

 

In my DMG mori DMU70 with Siemens 840d controller, I could move the fixture and still run the same program even without using RTCP/TRAORI (but with the use of Cycle800). Am I missing something?

[Rocketmachinist]

9 hours ago, Shiva.aero said:

Thanks for the link Rocketmachinist!

So in simple terms, in RTCP mode, the WCS or G54 is attached to the Part & move with it, instead of getting fixed to the machine or space.

Is that all or anything more to it?

 

                  The other thing it does is simplify programming. Especially if you are doing any of it by hand. Because it keeps track of that one point in space you can read back the numbers much easier. Say you are working on a part on a horizontal. You work on the front of the part and then you need to rotate the part 90 degrees and put in some holes. You can do that operation in 3 ways.

                    You can set a new work coordinate say g55. This method will let your numbers look the way they do on the print. So if you need to move to X1. Y1. to a hole depth of Z-1. Then you can read the numbers before you put in the hole. In this method, you have to set up a new offset in your control and make sure you are calling that offset in your program.

                   In the 2nd method, you let your cam do the work. In this method, you have to find the center of rotation, then find out where your parts sit relative to that center of rotation. Put those numbers into your cam and then run your parts. If you need to use any offsets it's going to get weird. Also, the numbers with all have those offsets added to all the numbers. So if you are drilling from a top of stock of 14. inches to a depth of 13 inches. That is the same as drilling from 0 to a depth of -1. This one only requires g54 one work offset but if any parts shift in the location you have to reprogram the whole thing.

                    The last method with TCP is a good combo of the two. You can use probing to set your parts if you want. You only have to touch one side of the part. The numbers in the program are very readable. Part shifting can be done on a case-by-case basis. The same program can go from machine to machine and doesn't need to be modified to the center of rotation of that new machine.

[Shiva.aero]

1 hour ago, Rocketmachinist said:

                  The other thing it does is simplify programming. Especially if you are doing any of it by hand. Because it keeps track of that one point in space you can read back the numbers much easier. Say you are working on a part on a horizontal. You work on the front of the part and then you need to rotate the part 90 degrees and put in some holes. You can do that operation in 3 ways.

                    You can set a new work coordinate say g55. This method will let your numbers look the way they do on the print. So if you need to move to X1. Y1. to a hole depth of Z-1. Then you can read the numbers before you put in the hole. In this method, you have to set up a new offset in your control and make sure you are calling that offset in your program.

                   In the 2nd method, you let your cam do the work. In this method, you have to find the center of rotation, then find out where your parts sit relative to that center of rotation. Put those numbers into your cam and then run your parts. If you need to use any offsets it's going to get weird. Also, the numbers with all have those offsets added to all the numbers. So if you are drilling from a top of stock of 14. inches to a depth of 13 inches. That is the same as drilling from 0 to a depth of -1. This one only requires g54 one work offset but if any parts shift in the location you have to reprogram the whole thing.

                    The last method with TCP is a good combo of the two. You can use probing to set your parts if you want. You only have to touch one side of the part. The numbers in the program are very readable. Part shifting can be done on a case-by-case basis. The same program can go from machine to machine and doesn't need to be modified to the center of rotation of that new machine.

Thank you very much Rocketmachinist! 

In the 2nd method you explained, by 'center of rotation' do you mean 'center of rotating axes'?

In 5 axis machines there are 2 rotating axes and which one is used in this method and how this center value is used?

 

[Rocketmachinist]

Yeah, the center of rotating axes.

 

For true 5x motion you would only use examples 2 and 3. Example 1 is only good for indexing, it doesn't lend itself to 5x.

 

For example 2 in 5 axis motion, you are letting your cam system do all the work. This method is totally fine but very labor-intensive when jumping from machine to machine. Every single program will only work on that machine. So if I have to go from a Haas UMC750 to a 5x Okuma, then the file will have to be modified. Because each machine's center of rotating axis is different.

 

For example 3 I could take the same program from a  Haas VMC 750 put it in an articulating head machine like a Haas VR-8. This is all because the controller is handling its own machine dynamics. It knows where all the axis pivot around. So the math is done in real-time by the machine. That's how you can take apart and put it where ever you want. Because the control is interpreting the program to whatever pivot distances it individually has.  That is why TCPC is so awesome.  

[cncappsjames]

On 11/2/2021 at 10:06 PM, Shiva.aero said:

In my ... Siemens 840d controller, I could move the fixture and still run the same program even without using RTCP/TRAORI (but with the use of Cycle800). Am I missing something?

Those functions you mention use the "Swivel Table". The Siemens equivalent to the FANUC #19700-#19705 parameters in a Table/Table type machine. This is what allows you to locate the part anywhere on the table, set the work offset and as long as your swivel table and tool offset is set correctly, you're good to go.

Personally, I'm not a fan of Center of Rotation programming. If you have a part geometry problem, it makes for a bigger challenge to determine the cause.

[Shiva.aero]

13 hours ago, cncappsjames said:

Those functions you mention use the "Swivel Table". The Siemens equivalent to the FANUC #19700-#19705 parameters in a Table/Table type machine. This is what allows you to locate the part anywhere on the table, set the work offset and as long as your swivel table and tool offset is set correctly, you're good to go.

Personally, I'm not a fan of Center of Rotation programming. If you have a part geometry problem, it makes for a bigger challenge to determine the cause.

For Table-Table 5 axis machine, since the tool is not going to tilt, why we should worry about tool offset?

Instead of using Cycle 800, if we use simply AROT or B(angle)/C(angle), then will there be any problem?

[crazy^millman]

4 hours ago, Shiva.aero said:

For Table-Table 5 axis machine, since the tool is not going to tilt, why we should worry about tool offset?

Instead of using Cycle 800, if we use simply AROT or B(angle)/C(angle), then will there be any problem?

CYCLE800 is really nice because you can have Zero at each datum structure on the part and all coordinates for the NC code zero from each CYCLE800 position. Without this then all numbers have to come from one Zero in the NC Code and when you get into 3+2 work sometimes it is nice when running and proving out the part for see numbers from each 3+2 position verses back to one place that can be very hard to sort out and see if they are correct. Just because the tool is not going to tilt to the different angles the table moving can create some odd numbers and values that would hard to double check. You have a 400mm shift at a 27.658 degree to a face and then have a hole pattern or feature called from it. Nice to see those values in the CYCLE800 line and then all depths and features nominally from that place to feel comfortable yes I am drilling 30mm deep at this 3+2 place. Your way would require numerous work offsets and possibility of error, but using CYCLE800 and letting the machine do what is was designed for those problems and issues are lessened greatly.

[cncappsjames]

5 hours ago, Shiva.aero said:

For Table-Table 5 axis machine, since the tool is not going to tilt, why we should worry about tool offset?

If your tool offset is wrong... let's say you have a 3mm thick floor and you use the same tool to machine the pocket and face off the back. Let's assume your swivel table is correct. If your tool is off by .5mm (too long) now instead of having a floor that is 3mm thick, you have a floor that is 2mm thick. That's why tool offset values matter.

CYCLE800 is better than the other methods you mention because with CYCLE800 your datum structure stays intact. With COR programming the numbers will be relative to COR.

[Leon82]

When you program off the datums and not the center of rotation are you shifting it when you go into Camplete? Otherwise a simulation is going to be cockeyed.