AnsweredAssumed Answered

Fadal CNC HS88 Posts

Question asked by Grace Watson on Apr 19, 2017
Latest reply on Apr 21, 2017 by Brian Suchland

Like • Show 0 Likes0
Comment • 6

The post for machine does not work like I expected it to. I might not have something set right but I didn't really change anything. I installed Cam and ran it with no changes. I took the output G-code to my favorite Master-cam programmer and said look at this. He had a few comments but was over all pleased. He ran a back plot in Cimco Edit with the program that I had output. These could be things only we use.

See comments:

Post has extra line spaces or carriage returns

Post missing % at beginning and end

No safety line for setting model options

Attachments

KTM950 emissions block off plate.txt.zip919 bytes

No one else has this question

Outcomes

6 Replies

Michael Buchli Apr 19, 2017 4:30 PM
Mark Correct
Correct Answer
Good afternoon,

Thank you for the feedback. I have a quick question. I am assuming you selected the FadalCNC post processor correct? It doesn't look like the Fadal post has this by default but I want to check.

The post processors that come with SOLIDWORKS CAM are generic and being worked on during the beta process. Similar to other CAM packages, users can also get custom or guaranteed post processors from certified resellers.

If you are looking for a custom post processor for your Fadal to test out CAM on a machine, please let us know and we will get a post that will work for your machine. The feedback you gave us will be added to the list for future standard post processors. Can you post a sample from a current program so we can see the layout that works for your Fadal?

Thanks Mike
Like • Show 0 Likes0
Actions
- Grace Watson @ Michael Buchli on Apr 19, 2017 4:49 PM
  Mark Correct
  Correct Answer
  Mike,
  
  I selected the FadalCNC post just as your picture shows. One of the most common and most sold machines of all time was Fadal with an HS88 control. Almost every machine shop in the USA has one or more. Their cheap simple and a very good place to start new operators. Also the Fadal uses E numbers for offsets but will recognize standard G54-59. https://itscnc.com/images/Program_Codes_2.pdf
  
  One other things I forgot in my original post. My center drill used a G82 with a dwell. This is very strange and not a good practice. It would have been better to have a G81 cycle for the center drill.
  "The post processors that come with SOLIDWORKS CAM are generic and being worked on during the beta process." What does that mean. Why do you have a selection for a control if it will not work?
  Like • Show 0 Likes0
  Actions
  - Michael Buchli @ Grace Watson on Apr 19, 2017 5:13 PM
    Mark Correct
    Correct Answer
    Thank you for the feedback and pdf file. One quick thought for the dwell issues is the Center drill parameters. By default I believe it is set to spot drill. Changing the parameter type to drilling should change the sub routine cycle that is called in the post to G81. (image 1) If you standard is to use drilling for center drills you can update the standards by using the Save Operation Plan button.
    
    If you go to the SW CAM feature tree and highlight the hole feature, you will be able to select "save operation plan" from the command manager or by right clicking on the highlighted feature.
    
    Once you are in the dialog, you will have the option to overwrite the existing rule or create a new one. if you overwrite the existing rule it will update the settings so the next time it is used, those will be automatically changed to your default. The rules in SW CAM control information related to tool selection and strategy parameters.
    
    Post processors and output can vary between controllers, settings, preferences and versions. When I mentioned that we are working the shipping posts, I mean that we are compiling information on the most common settings and versions used by the masses. When I last ran Fadals we had five mills and four of them would take the same post processor. One had different requirements due to the age of the controller. Your feedback will help us narrow down specific settings that should be part of the installation. Please let us know if you want an adjusted post processor to test SW CAM on your machine.
    
    Thank you again for all your feedback and have a great evening!
    
    Mike
    Like • Show 0 Likes0
    Actions
  - Shawn Patterson @ Grace Watson on Apr 20, 2017 8:16 AM
    Mark Correct
    Correct Answer
    Good day everyone!
    I would like to point out that you generated a program with very little edits that needed to be made....right out of the box. I too have a Fadal in my shop as well as 17 other machines. I also am a MasterCam user and needed to have all 18 posts individually edited by my re seller to make each control happy. Fadals are in about 40% of the shops I've visited or know of. Most shops that used them heavily are phasing them out for more productive equipment. I think the overall ease of use and being able to customize it to my individual usage is what I'm interested in seeing with this Beta trial. Just making an observation...so far I'm liking it!
    
    Shawn
    Like • Show 1 Like1
    Actions
Michael Buchli Apr 19, 2017 6:49 PM
Mark Correct
Correct Answer
Grace,

Good evening. I have taken your notes today and sent them to development to make changes to the Fadal Post Processor. When we get an updated version, I will send it to you so it can replace the current version you are using. I will let you know as soon as I have an update from the development team.

Have a great evening and thank you again for all your feedback!

Mike
Like • Show 1 Like1
Actions
- Brian Suchland @ Michael Buchli on Apr 21, 2017 4:40 PM
  Mark Correct
  Correct Answer
  Just an FYI on Fadal post processors....
  The Fadal machine was made available with multiple different machine controllers and the codes are different between them. Some of the rare controllers that Fadal machines have came with are Siemens 810D, Fanuc and the CNC 88 controller. The CNC 88 controller is by far the most common. However, the CNC 88 controller has TWO options of which to run the code. They are called Format 1 & Format 2. It is essential to ensure the correct Fadal CNC 88 Format post is used vs. the one that the machine is configured for. Essentially if the post was wrote for Format 1, and the machine is in Format 2.... you will have code issues.
  
  The primary differences are 1 format will support G54, G55 work coordinates etc. where as the other format will ONLY do E0-99 fixture offsets. Additionally some of the "machine home" commands are done differently. The tapping commands are completely different for both floating and rigid tapping between the two formats.
  Like • Show 1 Like1
  Actions

Fadal CNC HS88 Posts

Attachments

Outcomes

Related Content

Recommended Content