Why You Need an "Adaptive" Post

[jtreanor]

Hi Everyone,

Adaptive templates for posts -
In order to access the latest functions in Edgecam
you need to have a post based on an "Adaptive" template.

that's why the latest releases don't install all those old posts anymore.
If you right click - Edit your post (.mxt) source code file
it shows the template name the Code Wizard post is based on
with dates and development history.
If it doesn't say Adaptive you should plan on creating a new post.

Your Post controls many of the menu options and cycle dialog boxes

If you have an "Adaptive" post the spindle control and
coolant functions are now part of the Tool select dialog.
Compensation control is included in the profile cycle.
and new M-functions like "Update Stock".

Every release Edgecam is adding to and improving the core software.
to access and use the latest functions you need an adaptive post.

Caution: If you run .PCI's they will need to be updated
to include the new modifiers/options available in the cycles.

I'm sure I haven't touched on half the reasons or explained them very well.

[jpike10]

So to get the full benefits of the new releases i will need to update all of my posts, i have some that go back to 2005.
i also notice that the tokens have changed. once i have a new template built,
should i save it over the old one?
this should be fun ...i have a few custom posts

[jtreanor]

Hi JPike,

Try selecting one of the newer "sample" posts that ship
on the DVD, you will be able to see the new functions and
test any PCI / macros. and decide if there is anything new
that has value for you.

I wouldn't recommend overwriting your old post until you are sure the
new is working.

If you use PCI's it is almost certain they will need to be updated
to work with the new post, and once updated they will not work
with the old post.

I recommend you start a NEW Code Wizard.cgd post selecting
an adaptive template, then open a second window of Code Wizard
and side by side on screen copy the Formats, NC Style, and constructors
to match your old post.

you will find additional tokens in some of the constructors that may simplify
some of the older customization.
and yes, a few of the Token names have changed.

If you have custom code written in the "Warnings" constructor
it can be moved to the "Customization Whiteboard"

open a .ppf file (generate code) and use the Re-Run button
in Code Wizard to regenerate the NC code with the new post
until it looks the way you want.

Then again - what is your time worth
You could contact your Edgecam resource, give them your old post,
.pci's and .mac files and let them up do the upgrade.
I assume most Edgecam users aren't doing this for fun.
It is a business decision to make an investment in the upgrade.

[Tony the Ferret]

Wow..... What a carry on, so you can continue to use your software. Whilst you are on support with WorkNC, you can get your posts from your friendly Sescoi office. perhaps you should give them a call

[jtreanor]

Hi Tony,
I am a CAM user / programmer, not a sales or marketing rep.
Thats why I contribute to this forum.

My company pays for Edgecam and I use it. (for the last 15 years)
If I have the time I write and update my own posts and automation.
Sometimes I hire someone to do it for me.
My real job is making chips (swarf to you).
What's yours ???

[Tony the Ferret]

Hi
Yes i was like you in a previous life, programming and cutting parts, i worked in various factories (shops to you, we buy food from ours) press tool, mould tool and also general machining. Both from CAD CAM and manual programming with Q-defs on Heidenhain controls,
I have never needed more than 3 posts to complete all my work. Since working with WorkNC, i do not have any customers who have a NEED for more than one. I could not imagine programming a complex job and thinking HUM... Hum, wonder which post will do the job for me,, could it be ......987,,, or perhap the good old one 103... Oh no not that one it was compiled for 3 versions ago, and that will gouge.. Should i try XXXXX.
By this time my boss would have been jumping about,,, where is my %$E^&y job. either get cutting or get your coat.
I was only asking, why someone would need to go to all this trouble and have many posts, the software does all the hard work, why make life complicated, Just have ONE postprocessor that does it all.....

[jtreanor]

Hello Tony,

So the answer is - you are here trolling an Edgecam
help forum trying to get some business for yourself.

Since this is the Edgecam forum I will enlighten you.

Edgecam posts are specific to each machine.
The post contains the actual machine graphics to allow
for full machine simulation, validation and collision detection.
If a tool gouges the part, you get to see it.

Each post defines the type and capabilities of the machine.
Lathe, Mill, Wire EDM, Router, Water Jet cutter etc.

If a lathe doesn't have Y axis or live tools you are not
able to select them, and if it does the post will output
all the correct M & G codes specific to that machine.

How can "one post fits all" know the difference between
a pallet change for a Haas and a user M-Code to initiate
an automated Robot load / unload cycle.
for Fanuc, Seimens and Heidenhein ?

A well written Edgecam post generates code that
requires NO edits, WYSIWYG
it goes straight to the machine.

I'm sure you are very proud of and happy to use the software you sell.
please let me know if you would like some help with Edgecam.

[Tony the Ferret]

Hi
Of course you are right, i would not expect a lathe post for work for a hass mill centre, or a heidenhain 155 to work well for a fanuc. I thought that was obvious to any one with a little sense.
I have only programmed for mills, and i still maintain that a post i wrote for a Heid 407 in 2000 will still work with the current version of WorkNC today. Without recompilation. As for gouges, we dont show those, because WorkNC does not have a button for "no gouges" that is automatic.

I am not interested in trolling for customers, as you can see, i an 100% UK, and have no interest in trying to get USA customers, I like to see what other software users are upto and what is good/bad. That is the whole point of a forum, to discuss in an open and frank communication, without upsetting anyone, if there are strong feelings one way or another. that is a forum.

My reason for looking on the edgecam forum is to see how other users judge the software. I know some EX and current Edgecam users in the UK and i want to service them better.
Tony

[jtreanor]

My Apologies Tony,

We are mis-communicating,

My OLD posts from the 1990's still work.
but they can't take advantage of the latest software capability.

example, Edgecam roughing cycles are semi-intelligent
the software knows what is stock and what is the finished part.
it removes the stock up to the offset value wherever the tool will fit.

NEW function in Edgecam - "Update Stock" so the next tool knows
where the remaining stock is and doesn't cut air.
and checks tool / holder / stock collision against the "current" stock

In order to get all the new functions you need to update the post.
normally this is just a quick 30 second update button.

But if you have OLD posts they cannot be Auto updated.
you need to start a new post from scratch using what
Edgecam calls an "Adaptive" post template.

the "Adaptive" post templates have been around for 5-7 years
if your post is older than that it needs the one time upgrade.

[Tony the Ferret]

Hi, you have me even more confused now ?
Why does the re-maching function in the software have an impact on the output to the machine, the control does not know what a remachine or raster finish does, it just follows iso code generated by the CAM software.
Reading some of the other posts on the edgecam forum i see several references to tokens and outdated tokens and even new tokens.
Sounds more like roulete
All i know is that my software on the screen creates the toolpath, i can view it, edit it, simulate it all without postprocessing; and fast calculations at that.
WHEN I AM happy with the results i can see, i THEN choose which machine the code will go to, can even change the axis system at this stage, because the muppet on the machine has put the job the wrong way round. the toolpath will not need re-calculating, only the output to the relevant control.

[jtreanor]

Hi Tony,

I guess the word "Postprocessor" is partially incorrect for Edgecam,
the Edgecam post is not a 3rd party or separate utility,
it is integrated with the software, In Edgecam you choose
the machine first, as I said the machine graphics are in
the post and while you are creating toolpath it is displayed
with the machine on screen, fixtures, vises, indexers, toolholders
are all visible while you are creating toolpath.

If you select a 250mm long drill you will see if there is interference
with the part or fixtures immediately.

In Edgecam you do not (usually) type in move commands or coordinates,
you select a tool, then select a process (rough, profile, groove, hole, tap, bore, etc) to be performed on the part.

because it is integrated with the software the post also controls
the displayed menu options, So if you choose a horizontal mill
with a pallet changer there can be a menu option to perform a pallet change,
If you select a dual turret lathe the available instructions are
different than a mill. If the post is defined that the machine does not
support Rigid Tapping that option will be greyed out.

When the machining process / instructions are complete.
You run a full machine simulation, and compare the finished
part with shape of the remaining stock to see if you missed anything
or gouged the part. The comparison is color coded, Green is
machined within (your) set tolerance, Red is gouged, Blue is stock
that was missed.

You can change / reselect the machine (post) but only machines
with similar capacity will be displayed. So your instructions for
a dual turret lathe cannot be "posted" to a mill.

If everything is good, push the "Generate Code" button.
If you didn't see a crash - there isn't one.
feedrate 100% - hit GO
Provided the operator puts the tools in right side up.