PathPilot v1.9.8

PathPilot v1.9.8 is now available for download from Tormach.com
In This Version-

Enhancements:
• Mill - /Lathe - Work Offset Table editablity.
• Ability to add images to comment lines when:
o a comment is on a line containing M00 or M01 AND contains a file name ending in .jpg or .png
o Please see Release Notes for PathPilot® v1.9.8 for more information.

Bug Fixes:
• Mill - Converstaional tapping hole pattern bug fix
• Mill/Lathe - MDI: Up/Down arrow bug fix
For release notes and more information on this version as well as issue tracking and reporting visit the PathPilot Software Center.

"• Ability to add images to comment lines when:
o a comment is on a line containing M00 or M01 AND contains a file name ending in .jpg or .png
o Please see Release Notes for PathPilot® v1.9.8 for more information."

This could be cool and very usefull. I have a computer and screen across the shop that I use for just this purpose. I can check screen clips of cam simulation I take to check fixture placement and part orientation.

Nice to see it in code window at certain points.

I installed 1.9.8 on a test machine and am running it in SIM mode since I don't have a spare Mesa card.

Testing the .jpg stuff gives somewhat flaky results. Some files are resized and display perfectly while others are ignored. I haven't yet determined the difference between working and non-working files.

The release notes say "For more information on programming with comments, refer to chapter 7, Programming." The newest manual that I can locate is from September and doesn't mention JPEGs.

BTW, the pictures display in the path display window rather than the code window.

I was thinking about this after my Post above. I do almost no code editing. I would need to setup a section in sprutcam to create a spot to code the jpg links. Not all that hard to do. My problem is I compile and recompile all the time I tweak settings all the time. Having to reconnect the picture links would be to much work, Unless this is for a very refined program.
Currently I take a series of cam sim screen captures named simply part-name-01- 0? Put in a directory for that part and in shop I can quickly look at screen and thumb thru stock size needed and setups required for each step. Saves me many steps back to my studio.

Still might be a nice option to use from time to time.


Edit: Just installed updated and made some parts. :)
Loaded a go to part program that is small, "most my parts are tiny", no mess, Easy 5c setup, That I use for 60% of my work.
Few minutes later I have a couple precision metal things.

Something I would like to see is a way to save all the items you have edited in the previous version. Re editing is a kind of a pain each time a new version comes out.

table travels, rapids, spindle delay, to name a few.

of course this does sharpen a persons editing skills..........

edit: X and Y travel limits remain unchanged after updating!

Looks like v1.9.8 also fixed my PP bug report Issue 1353, Mill - Conversational: Circular pocket routine can result in straight plunge on G code with small helical entry. There was no mention of this in the summary but they changed all the conversational preamble use of G64 from "G64 P x.xxxx Q 0.0010" to "G64 P x.xxxx Q 0.0000".

Don’t know exactly the side effects of this difference but where the conversational used to plow into the work piece with certain values entered, it no longer does this – that’s good.

However, I still don’t like the behavior it has when milling circular pockets that are close in diameter to that of the tool. So I applied my fix to it described here - Conversational Pocket Bug?

Is there a link to the v1.9.8 update please? Can't see it yet on Tormach's website.

Cheers, Andy

https://www.tormach.com/pathpilot-up...and-notes.html

Many thanks - I had to clear-out my cache to get the updated page......

Cheers, Andy

rdsi,
Did you get any response from Tormach regarding your "Conversational Pocket Bug" findings? Specifically related to the G3 code generated as the diameter of the pocket gets closer to the diameter of the tool?

Using the conversational, (ver 1.9.8), I set a circular pocket 0.375 in diameter using a 0.25 endmill. I indicated a total depth of 0.2 inches, with a DOC of 0.05 inches, a feedrate of 15, with a Z-feedrate of 10, and a stepover value of 0.0, (perimeter cut only). The conversational seems to add a G3 finish cut, so I would have expected the code to have generated a 5 pass helix at a feed rate of 10 ipm, but instead it created a 16 pass helix, (15 helix passes and 1 finish pass), at a feedrate of 5.0, with an DOC of 0.0137 for the helix cuts. So basically the DOC, (0.05) and feedrate that I entered in the conversational are getting re-calculated to be much smaller values. It looks to me as though PathPilot is doing this to try to match some calculated helix angle, (in this case 2 degrees), within the distance one full 360 degree pass. Is that what you are saying as well?

I've been running into this problem for a while with pocketing, and I have just been editing the G-code to get the results I want, i.e. in this case, I just go in and set the feedrate to 10.0 and set the "P" value of the first G3 line to 4 instead of 15, and that seems to work fine, but again, I was curious to know if you had heard anything back from Tormach.

Thanks,
GenInt

I filed a bug report mainly about certain values causing the tool bit to plow down to Z end without doing any of the helix cuts. This was listed as “PP bug report Issue 1353, Mill - Conversational: Circular pocket routine can result in straight plunge on G code with small helical entry” but has since been removed from their website since release of v1.9.8 which fixed the problem.

Tormach did send me an email about the problem being fixed in v1.9.8 but offered no explanations.

But, I still don’t like how it behaves when the tool diameter approaches the pocket diameter as I explained in this post: Conversational Pocket Bug? In topic #7 of this post I offer a fix to this behavior that one can apply easily and is in the attached zipped file. This fix will work on all the latest versions including v1.9.8 & you can undo the fix if necessary. Updating will clobber this fix so you would need to reapply it.

Quote:

---

Using the conversational, (ver 1.9.8), I set a circular pocket 0.375 in diameter using a 0.25 endmill. I indicated a total depth of 0.2 inches, with a DOC of 0.05 inches, a feedrate of 15, with a Z-feedrate of 10, and a stepover value of 0.0, (perimeter cut only). The conversational seems to add a G3 finish cut, so I would have expected the code to have generated a 5 pass helix at a feed rate of 10 ipm, but instead it created a 16 pass helix, (15 helix passes and 1 finish pass), at a feedrate of 5.0, with an DOC of 0.0137 for the helix cuts. So basically the DOC, (0.05) and feedrate that I entered in the conversational are getting re-calculated to be much smaller values. It looks to me as though PathPilot is doing this to try to match some calculated helix angle, (in this case 2 degrees), within the distance one full 360 degree pass. Is that what you are saying as well?

---

Kind of, the fix will do what you want, 4 passes, plus a final clean-up at the bottom. This is how I think it should be. However, you do want to dial the feedrate down as PP does because of the tighter angular movement. So when using GW use the standard feedrate calc – you don’t need to recalculate with Interpolate because PP is going to do it for you!

Quote:

---

Originally Posted by mountaindew

I was thinking about this after my Post above. I do almost no code editing. I would need to setup a section in sprutcam to create a spot to code the jpg links. Not all that hard to do. My problem is I compile and recompile all the time I tweak settings all the time. Having to reconnect the picture links would be to much work, Unless this is for a very refined program.
Currently I take a series of cam sim screen captures named simply part-name-01- 0? Put in a directory for that part and in shop I can quickly look at screen and thumb thru stock size needed and setups required for each step. Saves me many steps back to my studio.

Still might be a nice option to use from time to time.

---

MD - Have you looked into using the Toolpath Template feature in SC 10? It looks like that could be an easy way to inline comments to an operation. So long as you don't change the comment, it should show up in line no matter how many times you re-compile the G-code.

Quote:

---

Originally Posted by MichaelHenry

MD - Have you looked into using the Toolpath Template feature in SC 10? It looks like that could be an easy way to inline comments to an operation. So long as you don't change the comment, it should show up in line no matter how many times you re-compile the G-code.

---

Yes that does work using the comment function in toolpath template to generate the correct code format and can be arranged in sprut operation tree as desired . Just needed to be careful and use a standard directory tree structure to organize tap and igs files in logical directories that are easy to copy onto pp controller drive. Also set easy standard names like p1.igs, p2.igs in sprut toolpath template comments and they link up with minimal editing.

Sorry to hijack - as it seems there's a thread around elsewhere regarding this issue.

Finally spent time to get wifi up and running (Tormach adapter). Works - but if I write over any existing file (whether file is currently loaded or not), crashes the PathPilot controller. Run 1.9.8 (downloaded and installed this morning).

Is there a known fix?

WW