Generic 5 axis post + Machine Def

[jaydenn]

Afternoon,

I've been away from Mastercam for nearly 10 years, but now I'm back.

 

I'm having difficulty finding threads, posts, documentation, or anything for that matter that describes Machine defs, posts, and how the two relate.

 

I'm currently trying to set up a vertical 5 axis mill(B & C table-table) to do ONLY 3+2 machining(and it's proving to be very difficult due to complete lack of any technical documentation).

 

I have some questions;

1. Does the machine def serve any function at all? I can completely change rotary limits and it doesn't affect the posted output at all. I can change the fundamental kinematics of the machine and it doesn't affect the posted output at all. Is this a limitation of the generic 5axis post? Perhaps there is a switch somewhere to turn on the functionality?

 

2. When creating a Tplane for rotation, do the X&Y axis play a role in determining the B&C output? If so, how and why?

 

3. Could someone explain how the Tplanes are expected to relate to real world machining? Is there a document somewhere describing it?

 

Thanks in advance for any help. I'm sure there will be more questions before I'm through.

 

Jay

[Colin Gilchrist]

Hi Jay,

 

You are coming up against the limits of the Generic Fanuc 5X Mill Post, and how it was originally conceived. The post is "Generic" because there are variables that act as switches, and allow you to configure the rotary output and "type" of machine you are processing for. (Gantry vs. Head/Table vs. Trunnion)

 

Nothing for the Generic Fanuc 5X Mill Post is hooked up to the Machine Definition. There are many independent Post Writers that have created logic to read the settings in the Machine Definition, and use that information to configure the post output. The Gen Fan 5X Mill Post does not do this, nor is there logic to turn on any of that functionality from the Machine Definition.

 

You may be thinking this is a bad thing, but really, it isn't. There are variables inside the Post that you can change, and it will fix the output for the type of machine you are building. Just change the variables, and be done with it. CNC Software has a document that you might be able to get from your reseller that will describe how to change these settings.

 

Once you get the 'rotaxis' and 'rotdir' variables set, that will eliminate at least half of your issues.

 

For question #2, the XY axes typically do not play a role in creating your angle output. Only the Z axis vector of your tool plane is used to create B/C output. There is vector math to rotate the vector into the "rotary axis plane", and then resolve the vector with 'atan2' to get the rotary angle. This is the reason you cannot just "rotate Top" and expect it to rotate the C Axis of your output. It isn't designed to work like that. If a vertical tool vector is detected, a prompt will come up on the screen and ask you to enter the Primary axis angle. You can then enter the rotation for the first toolpath, and the coordinates will be shifted to account for this rotation.

 

For #3, again the plane is setup to prove the Tool Axis Vector. That is then resolved by the post to give you rotary output. There are Misc Values (integers) that can be used to control or "flavor" the NC code output, to account for some of the "generic" nature of the post itself. (that document I mentioned describes how to set these values and control the output.)

 

Hope that helps,

 

Colin

[crazy^millman]

When it comes to 5 Axis the outsider does a better job handling posts then the people that make the software. Kind of odd to have a machine definition for a post and tie every post to it, but not the 5 Axis one. Colin is pointing you in the right direction and getting the generic 5 Axis post documentation will help you if you are looking to do this on your on.

[jaydenn]

Thanks Colin,

Just knowing that the machine definitions have no effect is great. Why it's even a part of the software(as delivered), I'll never know.

Why deliver a post that doesn't integrate with basic software functionality? Seems like a major missed opportunity.

 

I'll focus my efforts on the post itself, and *hopefully* sort out the rotdir and rotaxis to get what I need.

 

 

Anyways, thanks again for the insights,

Jay

[Colin Gilchrist]

Hi Jay,

 

I can only give you my opinion, so take this with a grain of salt, but here is my take on the Machine Definition, and why it was not hooked up to all the generic posts:

 

The Generic Fanuc 5X Mill Post, in it's current configuration, was originally built when Mastercam Version 9 was still being used. The post was designed with logic that would setup all the internal math routines, and would generally "configure" the post output, without needing a Machine Definition file.

 

When the development of the Mastercam X series of software was developed, they created a Machine Definition Manager, with the idea of being able to build a machine "kinematic" tree, that tells the Mastercam Software itself, what combination of rotary and linear axes the machine has. Although it doesn't look at the rotary travel limits, Mastercam does look at the type of toolpath you have created, and what rotary axes would be necessary (A, B, or C) to produce the motion. So if you create a 4X Vertical program, and then try to switch to a Horizontal machine, or you have a 5 Axis toolpath (that requires 5X motion), and you try and switch it out with a 4X machine, you would get a warning.

 

So with the release of Mastercam X, CNC Software had to choose what received development priority. Do they fix the old stuff, or work on the new stuff? Some of the post (4X) were updated to read some of the values of the rotary axis component, and use that mechanism (machine def) to drive the post output. The main issue is that it takes a lot of post development time to add that logic into a post processor. More that you would guess just by looking at it, at first guess.

 

It would be damn near impossible to take the Generic Fanuc 5X Mill Post, as it exists in its current form, and add logic to read the machine definition, and just "figure it out" as to what your specific configuration of 5X Machine is. I saw a study from a machine tool builder once that attempted to study every type of conceivable 5X machine configuration that was currently on the market. There were something like 216 or 218 different configurations of 5X machines. So trying to build logic inside a post that could figure that out, is tough at best.

 

The solution of course is to build individual 5 Axis post processors, that are configured inside the post to be run with a specific machine configuration. Then the post can be setup to properly read the Machine Definition components, and setup the post output based on the settings inside the Machine Definition. There are plenty of 3rd party post developers that do exactly this. They write their own logic, and use the tools provided by CNC Software as a "base" to build off.

 

Why don't they just hook this all up for everyone, so it works "out of the box"???  -> My answer in a single word: Piracy. There are already plenty of software pirates out there, using Mastercam to make parts without paying for it. If CNC Software just included working machines/posts with the software, it would make software pirate's lives even easier. By only including some "generic" posts, they can almost guarantee that will force most legitimate customers to contact their Reseller to get a working post. That provides a source of revenue to the Reseller (they love to sell you stuff right?), and also make sure that a pirate has to search around to find a post processor, and in the process might out themselves as a pirate to someone who would report them.

 

CNC Software has never really wanted to be in the post processor business. They want to sell Mastercam, and let you work with your Reseller to get a working post processor for your machine(s).

 

The bottom line is that the Machine Definition and Control Definition files work beautifully, if you take the time and have the knowledge, to hook up the MD/CD to the post. There are many different Post Developers that do this. They have a solution available right now, today. It isn't "free" though, and in my opinion, it shouldn't be. Making a post processor is hard work. It takes time, energy, and skill to do it right.