I am trying to create a post for spiral pockets around a cylinder. everything works fine except for F9999.9999 which momentarily stops feeds on both X and A axis. I have attached the post below. I also just downloaded the most recent post processor for Tormach mills with same result.Any help would be greatly appreciated.
Thanks
Try this one
Thanks Daniel,,
I tried the Post processor in the link. i still had the same issues. What I ended up doing was deleting the lines with F9999.9999. Runs smooth as silk. I am completely new to all of this so this was a great learning opportunity. Not sure if what i did was the right way to correct the problem but it seems to work.
Thanks again
Britt
There seem to be some problems happening with pp they get some problems fixed and new ones pop up, once ADSK have there 1100 up and running things on there end should get better
Hi @bwcrifles
Thanks for posting! I believe you may be able to avoid this issue by changing the maxInverseTime variable in the post processor from 9999.9999 to 2000. This will limit the maximum inverse feeds posted by the post processor, which will mean that the fastest time a move will complete in is 0.03 seconds, which should still be fast enough for any more.
To make this change, open the post processor you are using and search for the line that says;
var maxInverseTime = 9999.9999;
Change that line to;
var maxInverseTime = 2000;
Please let me know if this works to resolve this issue - if it does we will consider changing this variable in our generic post.
Paul
I'm using the latest version of the Tormach post processor in Fusion 360. I cannot find the line var maxinverseTime. I'm looking under both the settings and properties tab. Do I need to look somewhere else?
Thanks
Britt
Hi @bwcrifles
Thanks for the response! You need to look in the post processor itself. To do so, you may open the post processor with a text editor like Notepad++.
One easy way to do this is to download the latest version of the post you are using from the Autodesk Post Library, edit it in Notepad (or Brackets), and then upload it to a cloud library. I have attached a Tormach PathPilot post with this change made to this forum post - please let me know if you are using a different Tormach post and cannot find the maxInverseTime variable in it.
Hopefully this helps! Please let me know if you have any questions.
I made the change in the post processor. Both X and A axis are doing the thing as they did with 9999.9999. When I delete the lines it seems to work perfectly.
Thanks
Hi @bwcrifles
Thanks for the response! My previous instructions were intended to investigate a possible bug in the machine controller, but it does not seem that that is the case. Thank you for testing that for us!
For now, please continue to delete the F9999.9999 rates from the code. I will pass this behavior along to our post processor development team to see if they have any input and will keep you updated if I have new information to share.
Please let me know if you have any questions - I'm happy to help!
@bwcrifles Are you sure you tested the pp I posted, I have just had a look and it does not put out a 9999.9999 any where (you just need to post and check with a text editor to know this), And the one @paul.clauss posted does not do it ever, but the default one does.
@bwcrifles one other thing you can do is, do a new setup in cam and do your toolpaths again and post it back out, another tormach user had the wrap toolpaths go funny, doing a new setup was the only thing that worked There wrap path was in a hart shape
@paul.clauss These problems with the tormach posts has been going on since they got it changed it for smart cool and user selecting the Axis of rotation.
Get the Boston crew to check it on there tormach.
Hi @daniel_lyall,
Thanks for the response - I retesting and noticed that the post I attached for @bwcrifles does limit the feed to F2000. @bwcrifles - are you sure you posted with the right post?
@daniel_lyall - Could you clarify what issues you've been running into with the Tormach posts since the smart cool/ user selected axis update? I am happy to pass any information you have to share along to our post team!
@paul.clauss Hit up @xander.luciano He helped out on getting the post working on the very first one that smart cool was added to, It had G94 and G93 in it and it needed a feed attached to the G93 and there was none.
If you go by what's on there web sight it's wrong, If you look in the manual that's correct.
Whats on there web sight apply's to Mach3 not pathpilot (this is not your problem but it's making problem's) That's why I suggested getting the Boston crew to run anything over there machine, Just to double check it's all good since they have a 1100.
I 'll try starting over in CAM. The code runs just when with the deleted F9999.9999. 2000 was definitely in the code after i changed the Post Processor. I still had same issues. Hopefully this can be addressed because I will be doing a lot of wrapped tool paths. Thanks for all the help.
Hey guys,
I have 0 experience with Tormach controllers so I could be totally wrong here, but I think the max inverse time should be 999.9999 and not 9999.9999, or (1,000 and not 10,000). Even though that is a small small movement it is posting out, the value might be too large to be properly interpreted by the controller. I would try with 999.0 as a max inverse time (which I think is something like 1ms of movement) and see if that works. I saw a couple other places on google suggesting 2,000 for fanuc controllers, but not for any tormach controllers (pathpilot or mach3).
This would be a lot easier if there was a machine simulator I could download somewhere.
I attached a post processor with 999.0 as the max inverse time feedrate and verified it outputs correctly, so I just need someone to test my theory.
Thanks!
-Xander Luciano
@xander.luciano Ask the the guys in Boston (Boston version of per 9) to test it on there 1100.
Pathpilot is just Linuxcnc 2.7 with tormach's front end, tormach have 2 linux programmers working for them that did the 2.7 version and pathpilot, It is a lose version of a system from MIT I cant rember what that was called but it's where linuxcnc and Mach3 started from..
That post I gave him should of worked 2, Mach3 does not need inverse time
Daniel and Xander Luciano
I tried both of your processors and all I get is the number 1 and a blank page . my Previous post processor works except for the 9999.9999.
@bwcrifles I am just uploading a vid showing a few things to double check you already know or just don't know adding a post to your cloud and personal posts and showing what one fails and is good
Hi @bwcrifles
I have brought the issue you are experiencing to some members of our post processor development team, who would be happy to test out your code if you'd like to send me a complete NC file for the program you are running. Please send over the program if you'd like to continue researching this issue - I'm happy to help!
Paul
I am more than happy to do whatever I can to help resolve this issue. I have attached the complete pst with the F9999.9999 issues.
Thanks