Hello Guest it is November 13, 2019, 01:53:29 AM

Author Topic: Post processor for new CAM system  (Read 6991 times)

0 Members and 1 Guest are viewing this topic.

Post processor for new CAM system
« on: August 26, 2009, 08:39:07 AM »
Hi, I hope you can help me. I am creating a post processor to suit the Mach3 for a new CAM system to the market, SharpCam:  http://www.sharpcam.co.uk/

We have a technology that sits on top of the post that allows the user to configure simple properties to suit there machine. This means that one post can cover many machines that have subtle differences.

For example a see from the documentation that arc centres can be specified in to ways, incremental or absolute. This is a good candidate for a configurable property. The user can just selected their choice from a drop down box.

I have a few question that I hope some of you guru's would possibly be so kind to help me with!


This is by no means an exhaustive list:

1.   I note the G43 expects tool length offsets to be positive. G44 for negative offsets. Should a choice be given for both? Is it common for users to use G44.
2.   Should an M6 be output regardless of the machine, I note on the ‘General Logic Configuration’ dialog that the ‘Tool Change’ group box seems to cater for all scenarios even if the machine is not fitted with an ATC.
3.   Can a tool be pre selected?
4.   Do an M6 always return the Z axis to the ATC position or retract and stop for a manual tool Change?

Thank you very much for your time.

Julian

Senior Developer

SharpCam Ltd

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Post processor for new CAM system
« Reply #1 on: August 26, 2009, 09:32:38 AM »
1.   I note the G43 expects tool length offsets to be positive. G44 for negative offsets. Should a choice be given for both? Is it common for users to use G44.

I think most will just use G43 but better wait for others to comment.


2.   Should an M6 be output regardless of the machine, I note on the ‘General Logic Configuration’ dialog that the ‘Tool Change’ group box seems to cater for all scenarios even if the machine is not fitted with an ATC.

Shouldnt be a problem to have M6 in there at all times as it is dependant on the setting in General Config as to what will happen.



3.   Can a tool be pre selected?

Normally preselect isnt done but a user can if they wish write a custom macro. As the M call will be dependant on what the user decides to call the macro  then probably best not to have that option, unless however you can add an option for the user to input the M number. It will be in the format of M***P(Toolnumber here)


4.   Do an M6 always return the Z axis to the ATC position or retract and stop for a manual tool Change?

The M6 macro will determine what happens here.

Hood

Offline Dan13

*
  •  1,244 1,244
    • View Profile
    • DY Engineering
Re: Post processor for new CAM system
« Reply #2 on: August 26, 2009, 10:13:26 AM »
1.   I note the G43 expects tool length offsets to be positive. G44 for negative offsets. Should a choice be given for both? Is it common for users to use G44.

I had problems using only G43 for both negative and positive offsets, and I was not fancy about using both G43 and G44, since the CAM doesn't know the actual lengths of all the tools I use and it has no way to determine which command to use (G43 or G44) for each tool. Trying to fix it would mean a lot of unnecessary work and a lot of room for mistakes.

I edited my M6 macro by taking out the Z move after the conditional. Now I am successfully using the G43 command for all cases.

Daniel
Re: Post processor for new CAM system
« Reply #3 on: August 26, 2009, 01:59:47 PM »
Hi, thanks for the replies.

It looks like G44 is not that common, does anyone use this? Should I add this property for the sake of completeness?

Quote
Normally preselect isn't done but a user can if they wish write a custom macro. As the M call will be dependant on what the user decides to call the macro  then probably best not to have that option, unless however you can add an option for the user to input the M number. It will be in the format of M***P(Toolnumber here)

If I use M***P(Toolnumber) and allow a number to be specified is P the only letter that can be used?

Quote
The M6 macro will determine what happens here.

I guess then I should add the option the return the head to the tool change position in case the M6 macro does not do this?
Would you typically expect to see a G28/G30 Z0?
Is G91 in conjunction with needed as per Fanuc?

Thanks for your help

Julian

Senior Developer

SharpCam Ltd: http://www.sharpcam.co.uk
« Last Edit: August 26, 2009, 02:03:40 PM by Talyrond »

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Post processor for new CAM system
« Reply #4 on: August 26, 2009, 04:13:14 PM »

If I use M***P(Toolnumber) and allow a number to be specified is P the only letter that can be used?

From my understanding you would need to allow the user to specify the M number, for example custom macros are 100 and above so one user may wish to use M101 to write their preselect VB in, another may use M234 etc. So you would need to allow that to be entered.
So the preselect line would be something like M234P2.


I guess then I should add the option the return the head to the tool change position in case the M6 macro does not do this?
Would you typically expect to see a G28/G30 Z0?
Is G91 in conjunction with needed as per Fanuc?

Thanks for your help

Julian

Senior Developer

SharpCam Ltd: http://www.sharpcam.co.uk

I would write that into my M6 macro, what I would do is have
Code("G53G0Z0")
As the first part of my toolchange, that would move the Z Axis to the machine coords zero position but again not sure how others would do it.

Hood

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Post processor for new CAM system
« Reply #5 on: August 26, 2009, 04:29:05 PM »
Just wondering if you have any plans to do a CAM for Lathes? A decent reasonably priced CAM for lathes is definitely needed.

Hood

vmax549

*
Re: Post processor for new CAM system
« Reply #6 on: August 26, 2009, 08:23:33 PM »
M6T# is the proper syntac for a normal tool change(mill).

BUT IF you are running a look ahead HOTswap tool changer then you will need to preselect the tool T# ahead of the M6 call. The T# calls the Tool to the que then the M6 calls it active. Just like Fanuc.

So it depends (;-0 TP

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Post processor for new CAM system
« Reply #7 on: August 27, 2009, 03:29:12 AM »
Interesting, will have to refresh this subject with Brian but the m***p** was the way he said it worked to me, then again maybe we had our wires crossed.

Hood
Re: Post processor for new CAM system
« Reply #8 on: August 27, 2009, 09:28:58 AM »
Thanks guys,

I will give the user a choice to pre select both ways!

Hood, yes we do plan on a Lathe version, but we want to develop the milling until it is more mature before we do.

One last question, is rigid tapping available?

Julian

Senior Developer

SharpCam Ltd: http://www.sharpcam.co.uk

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Post processor for new CAM system
« Reply #9 on: August 27, 2009, 09:35:31 AM »
Look forward to lathe, Mill seems good from the quick glimpse I gave it :-) Dont want to download the trial yet as I am short of time and I presume it will be time limited?

No rigid tapping is not possible at this time, should be in the Mach Industrial version when thats done but unlikely to be in standard Mach any time soon.
 You can do rigid tapping at the moment if you have a servo on the spindle but it involves doing a swap axis so has nothing to do with a Post Processor as it would need hand coded I think.

Some people do tapping via a floating holder but that probably wouldnt concern your PP either?

Hood