Utilizing TCP G43.4 with Mcam??

[SydwazShawn]

I ‘am trying to figure out what is exactly needed to use TCP (G43.4) in Mastercam. I had read a few post about it and asked a few questions but still need help. What programming differences do I need to do, compared to programming a HAAS trinnion with inverse time?

 

I contacted Makino and below is what he had to say!

 

 

"I believe mastercam will work relative to toolpath generation....concern I would have is getting the proper post processor output from mastercam if Shields wants to utilize tool center point control style programming...which is something we would recommend for rotary axis contouring type motion on this machine.

 

If just 2+3 style machininig...conventional 5x programming setup with DFO can be utilized...which I would think mastercam can handle easily.

 

So it is more than just the cam software...it comes down to post processing and 5x functions the customer wants to utilize to drive the Makino D500.

 

I would see if mastercam can post process for tool center point control (G43.4) style programming for the machine described above?

 

I can answer more questions as they come up. Keep in touch."

 

 

We are thinking of having ICAM do a post and simulator for this machine. I am assuming they can get a post done that can fill these requirements that the machine needs.

 

I guess I do not understand how I am supposed to program Mastercam to use G43.4! Is it all in the post?

 

Thanks for any help! I’m pretty new to this 5axis stuff, so I will be asking a lot of questions down the road.

 

Shawn…

[Bruce Caulley]

MC can do it no problem. Just need to make sure the post is sorted is all.

 

Bruce

[SydwazShawn]

Hi Bruce, thanks for the reply!

 

What about (G68.2,G53.1)? Do you usually use these in 3+2 machining? Also this machine has 3-dementional cutter comp(G41.4,G42.4). Does the post take care of all this stuff if set up correctly?

 

Shawn.

[SydwazShawn]

quote:

---

What about (G68.2,G53.1)? Do you usually use these in 3+2 machining? Also this machine has 3-dementional cutter comp(G41.4,G42.4). Does the post take care of all this stuff if set up correctly?

---

Actually what I meant was when you do 3+2 machining (index then machine), is that when the G68.2, and G53.1 take effect? Also when using 3-dementional cutter comp, is this really just for swarf type toolpaths, or is it always commanded on for any full simultaneous 5ax toolpath?

[Ron Branch @ Verisurf]

Ok with G43.4 you are in essence programming the tools with out gague length and the machine is doing all of the too length comp for you. No big deal with Mastercam more of a post thing no big deal. Easily added by looking to the mill5$ variable.

 

Ok other codes do different things and thinking the G68.2 is the coordinate shift and need to find a post that has this done.

 

Other things all do different things and you might be better calling IN-HOUSE and getting a custom post. HINT HINT and in case you do not get my drift Call IN-HOUSE the post specialist.

[SydwazShawn]

Thanks Ron.

 

I think we are going to use ICAM for our post and simulation. I just wanted to make sure I tell them everything I need to have in the post and understand myself what the heck they are asking for.

 

I don’t have the machine till January so it’s hard for me to understand exactly what I am doing without playing with the machine.

 

Shawn.

[Guest CNC Apps Guy 1]

CAMplete does this.

[Greg Williams]

So does Vericut

[SydwazShawn]

quote:

---

CAMplete does this.

---

Doesn't CAMplete only really support Matsuura, and Robo drill?

 

quote:

---

So does Vericut

---

I checked into Vericut! Way to expensive for us.

[Guest CNC Apps Guy 1]

quote:

---

quote:

---

--------------------------------------------------------------------------------

CAMplete does this.

--------------------------------------------------------------------------------

---

Doesn't CAMplete only really support Matsuura, and Robo drill?

---

Those and Mikron. SHould have got one of those instead of a machine that there's only like 1 or 2 in the US.

[Greg Williams]

quote:

---

I checked into Vericut! Way to expensive for us.

---

true it is not cheap, But then again ICAM is not a give away either

 

Personally and this is just my preference. I would never run a program on a 5 axis machine without first checking the code in vericut or similar. A small error can make a massive mess

[Guest CNC Apps Guy 1]

quote:

---

...A small error can make a massive mess...

---

THAT'S AN understatement, ESPECIALLY when you buy a machine where there are only a SMALL handful AT MOST on the CONTINENT!

[SydwazShawn]

quote:

---

Those and Mikron. SHould have got one of those instead of a machine that there's only like 1 or 2 in the US.

---

Thanks for your input Kyle!

 

quote:

---

true it is not cheap, But then again ICAM is not a give away either

---

about half as much with a post!

 

quote:

---

THAT'S AN understatement, ESPECIALLY when you buy a machine where there are only a SMALL handful AT MOST on the CONTINENT!

---

I know this is you Kyle! Selway should just sell Mikino know and dump the Matsuura's! Their's a new kid on the block! Actually I take that back, Kyle is a good friend and I dont want to start talking crap!

[Guest CNC Apps Guy 1]

NOT Kyle... Guess Again...

 

quote:

---

...dump the Matsuura's!

---

 

I'm gonna call your boss and insist on drug testing cuz that's just CRAZY talk.. j/k

 

Seriously though, Matsuura 5-Axis machines kick @$$. Just ask someone who owns one. Yeah she may not be as sexy as the "new kid on the block" but she's got the kinks worked out unlike "the new kid on the block".

[SydwazShawn]

quote:

---

Yeah she may not be as sexy as the "new kid on the block" but she's got the kinks worked out unlike "the new kid on the block".

---

I know, I know Matsuura is a bad xxxx machine. There were differences that favored the Makino IMO, but the limited amount of machines built is definitely a strike against Makino.

 

But hey, I like my girls sexy and edgy, with easy access!!

[Guest CNC Apps Guy 1]

LOL

[SydwazShawn]

P.S I know your name is James! It sounded like Kyle was talking to me again about the cons! lol!

[gcode]

quote:

---

I checked into Vericut! Way to expensive for us.

---

I don't know what a Vericut post costs,

but ICAM will hurt you.. good stuff, but

definitely on the pricy end

[SydwazShawn]

quote:

---

I don't know what a Vericut post costs,

but ICAM will hurt you.. good stuff, but

definitely on the pricy end

---

Didn't know Vericut made posts? I think Vericut simulation was almost double the price then ICAM, and thats with the ICAM post and verification.

[MLS]

What machine is it?

 

A couple things of my opinion:

LINTOL Your post needs to handle it IMO if it is a nutating head or table/table rotary machine. 4-axis, not so much.

 

ICAM and Austin NC are both options for other post processors. I believe support is better with Austin NC while power is probably a bit better with ICAM.

 

If you have a machine with a ceramic bearing spindle, hitting one bolt and trashing the spindle will pay for Vericut.

 

As far as G43.4, my experience has been whenever the machine is in 5-axis motion, it likes lots of points/vectors. It does not need them on locked axis cuts so much as it does when it is swarfing. I have been on the switch to CATIA so I never really used the newer 5-axis toolpaths, but in the old toolpaths the best luck I got was turning on point generators based on an angular deviation. I think I defaulted at .1 degree for our Makinos.

 

Mastercam is perfectly capable.

[SydwazShawn]

It is a Makino D500.

 

The Makino guy said that it likes alot of point/vectors. It's alot smoother he said! He said it takes alot of processor speed to read it, but Makino can handle it.

[MLS]

I should have read it in your first post I suppose. Heh

 

So tool axis vectors that intersect with a 0,0,1 vector where it is transtitioning from swarfing one direction to another cause a potential problem the way any CAM system outputs CL data for a table/table or nutating head machine. The CAM system does not know what the rotary axes will do. The post decides this. That being said, this is the need for LINTOL in the post so you do not get a huge rotary and tiny linear move. The post needs to be able to break the rotary moves while maintaining the tip of the tool in the proper position else you will get the tool sweeping in/out of position.

 

Don't send anything out on the floor without verifying it with a gcode verification software IMO. I have heard of ICAM's, but never seen it in action so I can't say good or bad about it.

 

Sounds like fun.

[SydwazShawn]

I actually talked to a guy that has a D500 in there shop running ICAM. For a second I thought maybe you were him because they are in Wichita. He said it took a while but they have a nice post from ICAM. I just needed to figure out what everything means so I can give them my own specifications of how I want the post.

 

I had Makino look over the post specification form and they ended up filling it out for me today actually. Now I can get a formal quote from ICAM.

 

I'm thinking fun will be an understatement. It will be my baby, along with the 12 pallet stacker to boot!

 

P.S. What is Lintol? Line tolerance??

[MLS]

Lintol is an APT statement short for Linearization tolerance. Most other CAM systems use APT of one kind or another as opposed to an NCI file for CL data.

 

Basically when a tool swarfs from one vector to the next, the tip of the tool will not track in a linear motion, although you want it to. It will track in an arc or curve. So the function of LINTOL is to set a chordal tolerance for the post to recognize when the arc deviates from the linear path you want the tip of the tool to take and add additional points in so that it tracks closer to a linear path. I.E. break up the rotary moves and adjust the XYZ accordingly.

 

With a nutating head or table/table machine it has the potential to want to make a C-axis move of up to 90 degrees in a tiny linear axis move so as A-axis approaches 0(but not at 0) the potential is large for it to sweep around into a wall regardless of how many vectors the CAM system outputs. This doesn't happen all the time, but there is the potential.

[Guest CNC Apps Guy 1]

quote:

---

P.S I know your name is James! It sounded like Kyle was talking to me again about the cons! lol!

---

Just preachin' the troof! There's a saying, you can lead a horse to water...

 

 

quote:

---

So tool axis vectors that intersect with a 0,0,1 vector where it is transtitioning from swarfing one direction to another cause a potential problem the way any CAM system outputs CL data for a table/table or nutating head machine.

---

In which case you need to level the tool velocity. CAMplete does this.

 

quote:

---

The CAM system

does not know

is incapable of knowing what the rotary axes will do.

---

Fissed

 

 

quote:

---

...That being said, this is the need for...

---

an application like CAMplete.

 

quote:

---

...so you do not get a huge rotary and tiny linear move. The post needs to be able to break the rotary moves while maintaining the tip of the tool in the proper position else you will get the tool sweeping in/out of position.

---

MOST post processors are incapable of understang machine kinematics which plays a huge role in how the machine will act when it encounters a 0,0,1 situation. Makino footing the bill for that post Shawn? They SHOULD!!! I'm guessing you're going to be into it for around 10k depending on what other features (like the ability to build your own posts) you want.

 

quote:

---

With a nutating head or table/table machine it has the potential to want to make a C-axis move of up to 90 degrees in a tiny linear axis move so as A-axis approaches 0(but not at 0) the potential is large for it to sweep around into a wall regardless of how many vectors the CAM system outputs. This doesn't happen all the time, but there is the potential.

---

I've seen what's left of tools and parts when this happens and I can tell you it AIN'T pretty. Bent vanes, snapped tools or worse.