CAMplete

[RandleXX]

They say it does not require a post to work with Mastercam. It uses only the NCI to generate code. We are looking into this for a new 5 axis horizontal and of course I'm a little leery of this claim and wonder if anyone else here has had experience with it or has any comments.

 

Thanks

Randle

[gcode]

CNC Apps Guy is the the Camplete expert around here

[Joe788]

What machine are you looking at? The CAMPlete guy at IMTS told me they only offer it for Hermle, Mikron, Matsuura, and Nakamura. Are they expanding into other builders, or are you guys buying a big ol' MAM72-100H?

[RandleXX]

Thanks gcode.

 

We are looking at a new 5 axis Matsuura

[Oscar R.]

They say it does not require a post to work with Mastercam. It uses only the NCI to generate code.

 

To my understanding you still need to program your part in MasterCam using the generic 5 Axis machine def and post, then instead of posting from Mastercam you save an NCI file and open it in CAMplete and run it through the CAMplete process. The process being basically setting up your part, fixture, tooling, etc. exactly as it would be in the machine and verifing your program.

 

We just got a Matsuura MX-520 and it came with CAMplete. It's the first time I've used the software but after a few hours of training with CNC Apps Guy, it didn't take long to get something posted out and ready for the machine.

Currently the machine is in use with a long run of parts that wasn't posted from CAMplete so I haven't had a chance to run the full process, but should be able to with in a few weeks when production is done with it.

 

CNC Apps Guy is the the Camplete expert around here

 

Yes.

[kccadcam]

Been using Camplete on our MAM72-63V's (5-axis table-table verticals) for three years.....

 

Program everything in Mastercam from center of rotation, post out the NCI file,

open it in Camplete. It creates the NC code and you can simulate the machine and watch the code at the same time.

You can speed it up or slow it down step by step if necessary.

One the best features for five axis is the Optimization. It changes feedrates up to the maximum you define,

Reminds me of inverse time feeds but does it in inches per minute.

 

The machine simulation is fantastic, the only thing I'm still waiting for is

the ability to import an STL file and have Camplete actually show the model being cut..

Right now you can define basic stock shapes(block, cylinder, etc.) and show them cutting but we don't

usually have basic shaped parts!! The other issue is defining tools, you have to build your tool library twice,

once in Mastercam and again in Camplete to make everything match.

I would go off on Mastercam's way of defining tools and holders, but that's a whole other subject....

 

CNC Apps Guy is the the Camplete expert around here

Absolutely, James has been a HUGE help to me with the support of our Matsuura's and Camplete.

He is a walking encyclopedia on the machines and the software...

(still working on the 4 digit tool numbers James)

[kccadcam]

CAMPLETE

 

Here's an image from Camplete's website:

[Newbeeee™]

Playing devil's advocate here...so what is the difference between proving out in camplete (using mcam nci) or proving out in mcam's machine sim (using mcam nci)?

[Mic]

Playing devil's advocate here...so what is the difference between proving out in camplete (using mcam nci) or proving out in mcam's machine sim (using mcam nci)?

 

Camplete first postprocess the nci and the run the machine simulation on the posted nc-code. Huge difference.

[kccadcam]

Playing devil's advocate here...so what is the difference between proving out in camplete (using mcam nci) or proving out in mcam's machine sim (using mcam nci)?

Camplete first postprocess the nci and the run the machine simulation on the posted nc-code. Huge difference.

 

Yes,, Camplete post processes the NCI file and the NC code is what you are simulating.

You can click on any line of NC code in the NC window and the simulation will jump right to that point.

[Dtm]

I have heard good things about Camplete, but Vericut is supposed to be the best. What's the price difference between the two? I have used vericut on some jobs and you can import STL models for stock, but I also had to create my tool list twice. I'm no expert with vericut by any means, but it sure has saved me a few times when mastercam verify looked good.

[Newbeeee™]

Yes,, Camplete post processes the NCI file and the NC code is what you are simulating.

You can click on any line of NC code in the NC window and the simulation will jump right to that point.

 

So does this then mean that you need a specific camplete post per machine in your workshop (I asume this is a yes, as you would also have the whole machine built to match yours on the shop floor)?

And I'm then asuming if you want to edit that post for whatever reason, that's probably big bucks and only the camplete boys could do it?

 

Lastly, is this predominanly 5ax only that you would use this for, and or multiax lathies?

Thanks

[Dtm]

So does this then mean that you need a specific camplete post per machine in your workshop (I asume this is a yes, as you would also have the whole machine built to match yours on the shop floor)?

And I'm then asuming if you want to edit that post for whatever reason, that's probably big bucks and only the camplete boys could do it?

 

Lastly, is this predominanly 5ax only that you would use this for, and or multiax lathies?

Thanks

 

No you don't need a post. You just position your stock and fixture were they will be on the machine and set your origin. Then you run a verify just like in mastercam, but the difference is it will simulate the Nc program created from mastercam or any other cam system.

[kccadcam]

So does this then mean that you need a specific camplete post per machine in your workshop (I asume this is a yes, as you would also have the whole machine built to match yours on the shop floor)?

And I'm then asuming if you want to edit that post for whatever reason, that's probably big bucks and only the camplete boys could do it?

 

Lastly, is this predominanly 5ax only that you would use this for, and or multiax lathies?

Thanks

Yes, you need a specific "post" for each style of machine, and yes Camplete builds the whole virtual machine for each one.

The post IS customizable to a certain extent, I've got ours dialed in pretty darn good.....

Support has been very good... (I used to run Predator and they had the WORST support I've EVER experienced.)

[kccadcam]

Here's a screen capture of our machine, I run dual monitors so the pic is ....w i d e....

(hold down Ctrl button and scroll mouse wheel to enlarge)

 

Camplete screen capture

[Newbeeee™]

Thanks Kev - I understand now.

[Dtm]

Yes, you need a specific "post" for each style of machine, and yes Camplete builds the whole virtual machine for each one.

The post IS customizable to a certain extent, I've got ours dialed in pretty darn good.....

Support has been very good... (I used to run Predator and they had the WORST support I've EVER experienced.)

 

My bad. I assumed it was like vericut.

[MIL-TFP-41]

I was impressed with how customizable the "posts" are (CamPlete calls them NCFormats). They can interface with Matercam using canned text to set things up like tool breakage detection, high speed machining levels, ect. By no means could I control the output like I could in a Mastercam post, but I can say that it would always give me good results. Also it is capable of outputing more advanced functions like RTCP (or TRAORI on a Siemens controller), Tilted work planes, all that good stuff.

 

Basically....when you buy a Matsuura in the US, it comes with Camplete & the model of the machine you are going to drive. Buy a new/different machine...you get a new virtual model. One of the coolest features that I liked was I could take a program that ran on our V-Max800 5ax, change the machine to a MAM72-63V (totally different kinematics) and be able to run without ever going into Mastercam. To add to that you could go from a A-C machine like the 72-63V to a A-B machine like a 72-35V and do the same thing.

 

I agree that the optimization/linerization options in the software make it a must have......

[Mic]

One of the coolest features that I liked was I could take a program that ran on our V-Max800 5ax, change the machine to a MAM72-63V (totally different kinematics) and be able to run without ever going into Mastercam. To add to that you could go from a A-C machine like the 72-63V to a A-B machine like a 72-35V and do the same thing.I agree that the optimization/linerization options in the software make it a must have......

 

Small correction V.Max-800 5AX is AC table, MAM72-63V is also AC table, 35V is BC table

 

Only Matsuura AB so far is the huge MAM72-100H.

[Mic]

If you setup your fanuc nc-format with G68.2 (TWP) for indexing and G43.5 (TCPC type 2) for simultaneous, you could actually use the exact same nc-program on both AC and BC table kinematics.

[Guest CNC Apps Guy 1]

I have heard good things about Camplete, but Vericut is supposed to be the best. What's the price difference between the two?

Vericut is not a post processor, you'll need to have a post processor already in order to to use it. CAMplete does not have a machine builder module so you need to have either a Hermele, Mikron, Matsuura, FANUC Robodrill, or Nakamura. It is exclusive to those machines. There are no plans from my understanding to add any other builders' machines. Vericut can simulate custom MACRO programs, CAMplete at the moment cannot. CAMplete won't simulate tool breakage cycles, Vericut will.

 

Those are some biggies I know about.

 

The Vericut guys like to talk about CAMplete. I think it's because for the most part, every seat of CAMplete represents about a $15,000-$30,000 loss in revenue for their company and they are pretty pissed. Whatever... In my eyes, they are two VERY different products. Simulation and Collision detection is about the only similarities they share. We can do some things they can't, they can do some things we can't. The one thing for certain is, when you buy a 5-Axis Matsuura from us, you get CAMplete with the machine. You still have to buy Verict.

 

Hope that sheds some light on the differences.

 

Ont other thing that was mentioned that bears repeating... if you program a part for your MAM72-35V (BC kinematic) machine and you have say a 42V or 63V in the shop as well(both AC kinematic machines) , you can just change the machine, add in your new fixturing, you can move the program and part around to refelct the new setup (all from within CAMplete mind you) without ever having to do back into Mastercam. That's pretty darn cool if you ask me. SOmething I use CAMplete often for is to find out what is physically possible with a particular machine. We had a customer one time that had a part, if you thought about machining it in a conventional manner the part would not fit in the machine, no way, no how. Well, I sat down with them, in Mastercam we drew the machining envelope, so we had to rotate about X, Y and X to get it to fit in the envelope. I did a very basic fixture design to preove the concept, and I just did a Swarf profile around the part. All told about 30 minutes worth of work. Then I loaded the NCI file, the Part and the crude fixture and ran the simulation. If we ran the swarf and moved XY the machie overtraveled, so I set up the path to spin C axis and voila, no over travels. Had they not had and used CAMplete, they would have assumed they could not run that part in the machine.

 

HTH

[Guest CNC Apps Guy 1]

Oh, another plus to CAMplete ...

 

Traditionally, in Mastercam, if doing multi axis rotary programming, you HAVE to program the part from Center of rotation exactly like it sits in the machine... with CAMplete you don't. You can have that part oriented any old way and it doesn't matter. You just transform it in CAMplete to it's proper position and you're done. WHere this feature comes in especially anhdy is if you have a custom fixture made and it's different from the design, you can just shift things to make up for the difference. No need to go back into Mastercam.

 

Just thought I'd add that.

 

 

[RandleXX]

Thanks for all the input. Lots of good info so far..

[Mic]

Oh, another plus to CAMplete ...Traditionally, in Mastercam, if doing multi axis rotary programming, you HAVE to program the part from Center of rotation exactly like it sits in the machine... with CAMplete you don't. You can have that part oriented any old way and it doesn't matter.

 

With a good post from In-House or Cimco with support for TWP and TCPC you don't have to program from centre of rotation. Just put your work piece zero point on the machine in the same place as your mcam zero point and you're ready to cut.

[Guest CNC Apps Guy 1]

With a good post from In-House or Cimco

Cha-Ching...

 

with support for TWP and TCPC...

Cha-Ching... Cha-Ching...

 

CAMplete...

 

Included... AND it does G-Code Simulation unilke that MachSim stuff they are trying to push on us.

 

 

Just sayin'...