Re: Re: Post and INDEXER-LPT

>Message: 7
> Date: Wed, 17 Jan 2001 09:58:18 -0500
> From: ron ginger <ronginger@...>
>Subject: Re: Post and INDEXER-LPT
>
>Fred, can you elaborate a bit on the process of writing a 'post' Is it
>something one can do without the source code of the CAD system? What
>needs to be done, and how is it 'installed' into Vector?

Vector has a number of capabilities that allow the user to configure it for
both variations in machine and for user preferences.

1) The Contour, Cycle, and Macro menus contain a variable list of functions.
These can all be edited or removed, and new menu items can be added.
Each function can be altered to control the code that is generated, and text
can be interspersed with the generated G-code values. Contour and Cycle can
interact with drawing layers to produce.

2) Most G-code machines use the ISO001 driver. This generates a variety of
options that can be selected by checking radio buttons on the options dialog,
including, incremental vs absolute, modal Gcode and modal coordinates. There
are other drivers with Vector. One is the rotary driver which has the capability
to produce rotary axes output(angular), another is for the Agie Wire EDM machine,
another is for Heidenhein machines.

3) Coordinate decimals, fixed or floating field width, axis scaling are adjustable by
the coordinate settings, remove spaces.

4) Conversion- This is a sequential text substitution function. Strings on the left are
replaced by strings on the right, there are some complex wildcard and range matching
capabilities, identified strings can be reordered from the left to the right. (See the Lathe
configuration for some good examples)

5) Ask For - As G-code is generated a variable can be requested from the user in response
to it's placement in a Cycle or Contour.

6) Scripts - Up to 15 variables can be requested, math can be performed on the entries,
and input values, preformatted text, and calculation results can be placed in the program.
A good example would be to calculate the spindle speed and feed rate, given cutting speed
of material and drill diameter, the results can then automatically be written to the lines in
the program that have the S & F words called out. Scripts can be executed from the CAM
menu, or can automatically be called out in a Cycle or Contour.

A new configuration can be started by duplicating an existing one and giving it a new name.
This is done by clicking the new button on the insert NC dialog. By the time I review the
documentation of a controller, get a basic understanding of the requirements and syntax,
and configure a Vector setup, it takes about 3-5 hours, provided that I have one that is close
to base it on. Some machines have much more complex command sets than others.
Making a change to a configuration is immediately updated and the next time the setup is
used to generate, will be in effect.

Most of the underlying math of the actual output is not accessible to the user. The only time
that I have been stumped is on machines that are able to only identify an arc with beginning
and ending angles. Shopbot was like this at one time, and we simply interpolated the arcs to
lines inside the Vector drawing before generating the CNC code. This is another
configuration(Shopbot) to look at for some serious conversions. It produces comma delimited
coordinate values, as opposed to g-code.

Most of this is covered in the context sensitive help on the menus mentioned above, especially
the syntax for the conversions, scripts and ask for's.


Best Regards, Fred Smith- IMService
Listserve Special discounts and offers are at: http://209.69.202.197/cadcamedmdro.html

imserv@... Voice:248-486-3600 or 800-386-1670 Fax: 248-486-3698