Post processors for me spell daunting thoughts, lack ofknowledge and confusion.
So my objective here is to understand post processors. Ithink some info, answers to questions and an example or two lot of G code wouldhelp a lot.
Firstly it would be great to see a drawing of a basic partand g code produced for it using a CAM package, say call that g code example A.Then it would be good to see what would be changed using a post processorperhaps with the changed bits a different colour say example B. Then it wouldbe a huge help to understand the advantage for any changes.
I suppose here are my basic questions
1. Could what a post processor would edit be doneby hand in a sensible way?
2. What are the best and worst parts of a postprocessor and in which situation do they work best?
3. Is there a Post processor used for different CAMpackages or does a BobCAD one have to be used for BobCAD a Vectric one for Vectric software and so on, what Iwould like to know here is is there a universal post processor?
4. Is it that every time a CAM package is used apost processor has to be used?
I would of course welcome any help on post processors orgeneral help on getting going on a CNC mill. Some of you have already given great advice links and recommendationsand I would be further back still if I had not had them.
Many thanks in advance for any help.
All the best
Suesi there's no great mystery to post processors really they do a very simple job. There main function is to format the G-code file so it complys with the control software requirements.
Because in industry there are many different machines with different Control software from different manufactures each with different models that talk sligthtly different then you need a translator and that's the job of the post processor.
If CAM software didn't use Post processors then you would need a software version for each Model of Machine and Control software it used.
Often industrial machines come with there own proprietary CAM software which outputs directly to the control software in the correct format.
Now often these proprietary softwares are limited in what they can do or designed just for one purpose and it's because of this why Cam software often gets used has it's more flexible. To do this and work with many versions of control software the CAM software needs to Post processors designed for each control software model.
Now the Control software like MAch3 or Linux cnc are generic Control Software designed to be used with many machine types and designs. So in there basic form don't dictate any specific machine data be inserted in the G-code so a basic generic Post processor is all that's needed.
Most CAM software have Generic post processors which only insert basic G-code Initialisation lines such has setting Metric or Imperial units etc.
Now this can change if you have Machine specific needs or want your machine to behave a certain why. In this case you would alter or write your own Post processor to suit your own needs.
An example of needing to do this would be an automatic tool changer that needs a specific macro file to work. Here you would have the post processor define a constant in the header Portion(top of Code) that points to a file location then inserts this Constant at every tool change thru out the G-code file.
This way you can have Custom machines that all use the Same Cam software and Control software but are setup very differantly regards Hardware like Tool changers etc. You just have a Post processor written for that machine.
Often you'll see Metric and Imperial Post processors with the Only differance being Metric inserts G21 Imperial G20 the rest will be exactly the same.!!
To give an idea of Formated and unformatted G-code with specific and generic post processors I've attached 3 files all work with or formated for Mach3.
1st is from BobCad Cam.
2nd is from Solid works
3rd is just a Genric
Has you'll see the Formatted ones insert much more NONE G-code lines for information that gets displayed on the screen while cutting. They also do other subtle things like Setting the Initialisation of machine. So setting Work offsets and cancelling any previous Modal commnads or Canned cycles etc.
A simple Example of Post inserted Code is the Solid works Post processor Sends the Machine to the home location on all axis (G53) before starting the Main G-code.
Bobcad does the same but only for the Z axis and sets it 10mm away from home (G53 Z10). Bobcad also gives much more information about tool etc that gets displayed on screen but has no affect on the actual cutting.
The genric G-code does nothing really other than set Cancel tool length offset (G49) and set Distance Mode to Absolute (G90).
Hope this helps but in a Nut shell if your using Mach3 or Linux cnc don't worry about it and just use a Genric Post thats set for the units your using if you can't find a Specific Post.
The Following User Says Thank You to JAZZCNC For This Useful Post:
If you plan to buy a CAM package ensure your supplier will tailor a Post Processor for your machine as part of the initial support package, otherwise buy hardware and software that have a track record of compatibility.
Whatever you do you shouldn't initially worry about knowing how to write G-Code or Edit/Write Post Processors yourself unless you wish to provide support or help to others,
The Following User Says Thank You to magicniner For This Useful Post:
Once you understand the language of the post processor, it will become a learned language just like a spoken word, such as French or German, when creating post processors for various cadcam packages, I can picture exactly whats happening in my head, its quite fun really.
Many thanks for going to the trouble you did in trying to help I could not opensome of the files due to not having software on my computer. What you saidthough is really interesting to me.
All the best Sues
Thank you very much for the reply to my post. I am unsure what CAD CAM or justCAM package to buy. I only hope when I try some on a trial version the providerwill sort out a post processor for the trial version for my machine.
I am still trying to learn some G-Code and get going with my mill. You givegood advice so thank you very much.
Jazz has explained things in detail, but I feel he's missed the basics, which you may be struggling to grasp.
Essentially what your basic CAM package does, is create toolpaths. You load a drawing into the CAM, tell it what size the stock material is, select what tool you'd like to use, and it creates a suitable toolpath.
The post processor then tells the CAM how to output that toolpath in a format that your machine will understand, which for Mach3 is reasonably standard G-code.
If you want to try things out, I'd suggest downloading CamBam, as you can open the software 40 times and use it as much as you'd like, before any restrictions are put in place/you have to buy a license. CamBam also includes Mach post processors, and I'd also suggest you download the CutViewer demo as it gives quite a good simulation of how things will be machined, and highlight any issues.
By John S in forum General DiscussionReplies: 15Last Post: 01-12-2012, 04:56 PM
NEW MEMBER: First PostBy Jumbo in forum New Member IntroductionsReplies: 3Last Post: 17-10-2011, 12:58 PM
NEW MEMBER: Hello All, My First PostBy Harvey Wallbanger in forum New Member IntroductionsReplies: 1Last Post: 11-06-2011, 09:05 PM
NEW MEMBER: first postBy makinswarf in forum New Member IntroductionsReplies: 3Last Post: 08-05-2009, 01:44 AM
By m.marino in forum BobCAD-CAMReplies: 0Last Post: 21-01-2009, 11:37 AM