spacemanspiffee

Force XY move before rotary move

Recommended Posts

Hey all.

At work we have a Royce head head style large format router. We've got a Postability post for it that is somewhat old (I'm fairly new at this company) and works OK, but I'm still needing to do the same hand edits to every program. I'd like to eliminate that. Using this post, after a toolchange the Gcode moves the rotary axes before positioning the head over the workpiece where it will be cutting. This can sometimes cause errors on the machine of over axis limit travel.

We currently are hand editing the Gcode to move the rotary positioning moves after the first XY positioning move for every toolchange. I'd like to fix this in the post such that this sequence of events is followed:
1. tool change

2. machine moves to Z safe plane

3. machine moves to XY 

4. machine positions AB axes

I don't have very much experience editing post processors so I'm not sure what to look for and any help is greatly appreciated.

MPPOSTABILITY_ROYCE_8055.pst

Share this post


Link to post
Share on other sites

This post is not that old...I'd bet if you reached out to Postability they would handle everything you need. Their support is top notch

[email protected]

 

 

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

Be sure to send them a copy of what gets posted and a seperate file of the correction you need

good luck!

  • Like 3

Share this post


Link to post
Share on other sites

To add to this:

  • Dave sets up his Post Processors to allow you "control" over the events that take place.
  • You control the output of the Post Processor, by setting integer values for the Miscellaneous Integers and/or Real Numbers (decimal), for every Toolpath.
  • You can have Postability change the output for these options, to get exactly the code you want. But you'll still need to remember to open each of the Toolpaths, and adjust the settings, so that each approach/retract is handled the way you want it to be handled.

You will often have a choice of "0" = Option A, "1" = Option B, "2" = Option C.

In addition, there is typically another control that you can set for something like this: "1" = Only at real Toolchange, "2" = At Actual and Null Toolchange, Etc.

The idea is to give the Programmer control, so that you can adjust the "input" settings in Mastercam, and based on the changes you made, you get different output generated from the Post Processor.

  • Like 2

Share this post


Link to post
Share on other sites

I have a vague idea what you are talking about, but am unsure where I set the integer values. I am fairly new to MasterCAM (I've been programming in BobCAM for Solidworks for a long time) so I'm still learning where all the buttons are and what they do in relation to what I'm used to.

Can you explain this a little more for me?

Thanks!

Share this post


Link to post
Share on other sites
3 hours ago, spacemanspiffee said:

I have a vague idea what you are talking about, but am unsure where I set the integer values. I am fairly new to MasterCAM (I've been programming in BobCAM for Solidworks for a long time) so I'm still learning where all the buttons are and what they do in relation to what I'm used to.

Can you explain this a little more for me?

Thanks!

Sure, no worries.

When you program in Mastercam, you create a series of Toolpath Operations. You've probably figured that much out already, based on the fact that you are hand-editing the NC Code output.

When you create a new Operation, there are two potential "Operation Interfaces" that you'll see, depending on what type of Toolpaths you use.

If you mainly do 2D work, most of the 2D Operations have been re-worked in the Mastercam interface, to use a "Tree Style" Format.

On the left side of the Dialog Box, you'll see a Tree, where you select different "branches" or nodes. When you choose a new branch, it changes the display of the 'page' that is shown to you. Each page in the Op Tree contains different settings.

One of these pages, is called "Misc. Values". This page is a special page.

It is special, because it allows a "two-way flow" of information between the Post Processor, and Mastercam Ops.

If you look at the picture, you'll see I selected the Misc. Values page, and the settings are "grayed out". There is a checkbox that you must disable, if you want to use custom settings. Otherwise, you'll just be using the "Post Default Values".

image.thumb.png.948de0b9ed449abf7dde85dfc0a49f83.png

 

The "Strings" which are displayed in this page, come from the Post Processor Text Settings.

This gives the Post Developer, the ability to describe "what that control is going to be used for, inside the Post Processor".

These settings give you 10 Integer Numbers, and 10 Decimal (Real) Numbers, which act as "Input" to the Post Processor.

What can you do with them?    >>> Anything!!!

They exist in the program architecture as a way for the Post Developer to be able to "control events", based on the number that is being passed for each Operation.

This gives the user the ability to set different values, whenever they want a change to occur in the Posted code.

None of the Misc. Values are "setup by default", unless they were previously created for the "Base Post" which your Post Processor was created from.

Since you are using a Postability Post Processor, they have completely customized this section, to give you the ability to interact with the Post, and pass instructions to trigger different behavior, by manipulating the NC Code output.

Technically, there are 3 different mechanisms within Mastercam that allow the Post Developer and User to interact with the Operation Interfaces:

  1. Misc. Values - Passes numbers to the Post at the Op Level, to trigger routines in the Post.
  2. Drill Cycles - The "Cycle Text" and "Variable Descriptions" are editable, for each individual Drill Cycle. (20 different cycles available!) This allows you to completely customize the Drilling Cycle output, and/or create a "Custom" Drill Cycle. (For example, so you can add "Probing" support to a Post.)
  3. Canned Text - A special mechanism within Operations, that allow you to trigger events. And, since the release of Mastercam X, allow you to customize and control Coolant Output. Canned Text is "special", because you can use it "within the motion of a Toolpath", by using the "Change at Point" function in the Chaining Dialog. You can choose Canned Text output options (before, with, after) at the Operation Level (by default), but you can also do some really slick stuff with this function, since you can trigger events within a Toolpath itself. Misc. Values and Drill Cycles are only output at the "Tool Change" event.

 

 

  • Like 3

Share this post


Link to post
Share on other sites

Colin,

Thanks for the excellent explanation. I thought that the Misc Values page might have been what you were referring to, but wasn't sure.

This sounds like a pretty powerful way of getting the code output exactly how I want it.

Are all the Misc Values something that Postability sets up, or is that some thing that I can tweak myself? (obviously with enough know how I could make the changes myself, but like I said I'm new to editing posts and MasterCAM in general).

Does Postability provide documentation on what each of those values does other than the "strings" that are displayed on that page?

I appreciate the detailed answer!

For context as to myself, I'm new to MasterCAM. I used it for a few months in college in a CNC class I took doing 3+1 and 3+2 programming. I haven't used MasterCAM since then before starting this new job. I am not new to programming and running CNC machines. I started using BobCAM for Solidworks to program little desktop hobby machines toward the end of highschool, then graduated to tormachs at the beginning of college, and then got to do some work using Haas vertical milling centers, and recently got a 5'x5' 3 axis router for woodworking at home. I haven't had to do much post editing for any of those as the posts provided by BobCAM have been adequate for my needs. 

For work I'm now programming using MasterCAM on large 5 axis head head style routers doing simultaneous 5 axis stuff, which is a bit of a jump in complexity but is also pretty cool.

Share this post


Link to post
Share on other sites
1 hour ago, spacemanspiffee said:

Does Postability provide documentation on what each of those values does other than the "strings" that are displayed on that page?

Yes they do:

Docs Link

  • Thanks 2
  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us