Post Processor help for Centroid Mill Control

Having problems with or questions about SheetCam? Post them here.
Post Reply
Brian Lamb
Posts: 25
Joined: Fri Mar 02, 2018 11:04 pm

Post Processor help for Centroid Mill Control

Post by Brian Lamb »

Hi Les,

I recently converted my Milltronics CNC mill to a Centroid All in One DC Servo system. I was able to use my exiting post for the Milltronics, which I had cobbled together from a Mach3 post and a Fanuc post, with some help from you for a few things. But, it does some things I need changed and some things that still never worked for me and required a lot of hand editing. So, in the interest of doing less of that, I have a few questions.

1. When calling a new tool and it moves to the first XY position, I would like to have a move to safe Z level, usually Z.1" in my case, sometimes it does this, sometimes it leaves it out and it will feed from Tool Change position all the way to the first Z depth call at the specified feed rate, example, Z-.5 F20.

2. G02-G03 arcs, can we leave out the Z level unless it is changing (i.e. helical moves)? Also, if I or J are 0, can we leave them out? Currently I get a Z on every line and I's and J's of 0.0000.

3. Kind of related to the G01, G02 and G03, my feed rate gets reposted on every change from G01 to G02/G03. I would like these to be modal and only posted if they have changed. This makes it worlds easier for me to change a feed rate at the machine once for the whole tool instead of hundreds of lines of code with a feed rate listed on every line if I'm doing straight and arc cuts on a lot of profiling.

4. The "OnNewOperation" comments, could they be moved to be right above, or below, the Tool description line? Currently they pop up before the spindle off, coolant off and retract from the last tool. Not the end of the world, but confusing being four or five lines up from the actual operation start.

5. I'm using canned cycles for drilling, new control uses a G84 tapping cycle. Could on "Autotap" we have it output the Feed rate on the line above, and then the next line be G84 X-- Y-- Z-- R-- P--, now on my machine I use a Tension and Compression holder and I know when I tap at 1000 rpm I need P.8, so 8 tenths of a second of dwell for revering the tap. So either we need a dwell value in the tapping operations box or I can just default the post processor to P.8 and change it manually if I ever need to. Also, the X and Y values on the canned cycles first line need to be called out, so I believe that needs to be changed in the post to nonModalNumber? Currently if I have already moved to the XY position it leaves them out and then doesn't drill that first hole.

6. In regards to canned cycles, I almost always use G99 on the canned cycle call line and need G98 on the last position call of the canned cycle. Then right after that, I need a G80 to cancel the canned cycle. I've been manually entering all of those. I can edit the post to add G99 in front of the G83 or G84, but where/how do I get it on the last portion line and add the G80 after?

7. I can't find in the post processor where parking position is entered, but it's happening currently before my M05, M08 and M25 (return to Z0 for tool change), that can get a bit dicey if I have clamps sticking up. Would it be possible to move the parking position call to the line just above the M30?

I know, a lot of questions... but I really prefer the simplicity of Sheetcam and would prefer to fine tune it for a better post, especially as popular as the Centroid controls are becoming.

Thanks!
Brian
Attachments
Centroid Mill V1.scpost
(6.74 KiB) Downloaded 92 times
Brian Lamb
Posts: 25
Joined: Fri Mar 02, 2018 11:04 pm

Re: Post Processor help for Centroid Mill Control

Post by Brian Lamb »

Just bringing this to the top...Any help? Any ideas?
User avatar
Les Newell
Site Admin
Posts: 3661
Joined: Thu May 11, 2006 8:12 pm

Re: Post Processor help for Centroid Mill Control

Post by Les Newell »

Hi Brian,

Sorry for the delay in getting back to you.
Brian Lamb wrote: Sat Jun 22, 2019 4:26 pm 1. When calling a new tool and it moves to the first XY position, I would like to have a move to safe Z level, usually Z.1" in my case, sometimes it does this, sometimes it leaves it out and it will feed from Tool Change position all the way to the first Z depth call at the specified feed rate, example, Z-.5 F20.
Could you send me an example job file that does this. I can't replicate the fault here.
2. G02-G03 arcs, can we leave out the Z level unless it is changing (i.e. helical moves)? Also, if I or J are 0, can we leave them out? Currently I get a Z on every line and I's and J's of 0.0000.
This is a an error in the format string for the Z moves. In OnMove you have 3 trailing zeros and in OnArc you have 4. Fixed in the attached post.
3. Kind of related to the G01, G02 and G03, my feed rate gets reposted on every change from G01 to G02/G03.
Same again. You have to be careful to keep the format strings the same.
4. The "OnNewOperation" comments, could they be moved to be right above, or below, the Tool description line? Currently they pop up before the spindle off, coolant off and retract from the last tool.
This is because in some cases an operation may carry on from where a previous operation left off. It needs to start the new operation to find out if it needs to retract etc.
5. I'm using canned cycles for drilling, new control uses a G84 tapping cycle. Could on "Autotap" we have it output the Feed rate on the line above, and then the next line be G84 X-- Y-- Z-- R-- P--, now on my machine I use a Tension and Compression holder and I know when I tap at 1000 rpm I need P.8, so 8 tenths of a second of dwell for revering the tap.
This post has a dwell option.
6. In regards to canned cycles, I almost always use G99 on the canned cycle call line and need G98 on the last position call of the canned cycle. Then right after that, I need a G80 to cancel the canned cycle.
Done.
7. I can't find in the post processor where parking position is entered, but it's happening currently before my M05, M08 and M25 (return to Z0 for tool change), that can get a bit dicey if I have clamps sticking up. Would it be possible to move the parking position call to the line just above the M30?
Do that in Options->job options->parking. Either use a save Z position for parking or use the custom parking code option which gives you total control over what happens.

To install this post, save the attachment to any convenient folder on your computer then run SheetCam and go to Options->machine->post processor. Click on the 'Import post' button. Using the box that appears, navigate to your post and open it. You will have to restart SheetCam for the dwell optin to appear in your tapping tool definition.
Attachments
Centroid Mill V2.scpost
(6.66 KiB) Downloaded 90 times
Brian Lamb
Posts: 25
Joined: Fri Mar 02, 2018 11:04 pm

Re: Post Processor help for Centroid Mill Control

Post by Brian Lamb »

Hi Les, thank you for the reply. I have attached the job file and the .tap file for a rectangular nut that I just got done making. You will see that the first tool is a 3/16" end mill and the program tells it to move to Z.1 on N0140 (line 14) and then when the next tool is called, a 3/8 90º chamfer mill, on line N3410 it goes to Z-.065 at F30 after the first position move. This is what I run into, it should position, then rapid to Z.1, then continue on with a feed rate move.

This file also has canned cycles and you can see that they don't have G99 and G98, or the G80 to cancel them. I will upload your modified post shortly and see how it works.

Thank you!
Attachments
Flipstop nut test new post.tap
(15.48 KiB) Downloaded 66 times
Flipstop nut test new post.job
(33.11 KiB) Downloaded 72 times
User avatar
Les Newell
Site Admin
Posts: 3661
Joined: Thu May 11, 2006 8:12 pm

Re: Post Processor help for Centroid Mill Control

Post by Les Newell »

It took me a little while to figure out what is going on.
The post processor does not know anything about M25. Before the tool change it lifts to the clearance height. After the tool change it assumes it is still at the same height. After the tool change it moves to the cut start X,Y then should rapid down to the plunge safety clearance. Unusually you have the plunge safety clearance set to the same as the clearance height. As it thinks it is already at that height it does not do this plunge move.
The answer is to reduce the plunge safety clearance or increase the rapid clearance.

The plunge safety clearance is a safety factor. It is designed to protect the cutter if the top of your work is slightly higher than it should be or if there are some chips on the surface. The cutter rapids down to the plunge safety clearance above the cut start height then completes the move to the cut start height at feed rate. Generally 0.5mm/ 0.02" should be plenty.
Brian Lamb
Posts: 25
Joined: Fri Mar 02, 2018 11:04 pm

Re: Post Processor help for Centroid Mill Control

Post by Brian Lamb »

Hi Les,

I tried the new post, closer, but still some issues.

1. Still getting the lack of Z.1 after the first tool. See line 343

2. Still see a lot of multiple Z depths call outs when profiling around the part. It seems to list the Z even though it hasn't change from every swap from G1 to G2/3. See lines 93 vs. 94 vs. 96 and so on. Lack of feed rate callouts is greatly appreciated.

3. Canned cycle... The G99 needs to be on the G83 (or whatever canned cycle call) line, should look like G99 G83 X Y Z R Q F. The G80 didn't show up.

4. Tapping canned cycle. I set up a tool for 5/16-18, might have used the wrong pitch, but I just tried it again, said it was 18 TPI, it is outputting a federate of .0556, which would be correct for one turn, I need it for one turn times the spindle speed, it's IPm not IPR. I tried editing the tool and saying the pitch was .0556 and now the code shows F16.6667, which it needs to be roughly 55IPM at 1000rpm.

It is also outputting M49, G95 and G99 (before the G84 call on the G99), then after the tapping cycle I get a M48 and a G94. Then I have a strange F3.937 just before the go to safe parking position.

5. In regards to the safe park, are you suggesting I write into the box "Custom Parking Code", something like this:

M25
G00 X16 Y2

And that would make sure I get the M25 first? I currently have the use X and Y boxes with 16 and 2 respectively, with nothing checked for Z and yet it puts in a Z.1, which is Z.1 above the Z0 of the part.

I hope all of that makes sense.

Thank you!
Attachments
Flipstop nut test new post V2.tap
(14.95 KiB) Downloaded 76 times
Flipstop nut test new post V2.job
(33.41 KiB) Downloaded 48 times
Brian Lamb
Posts: 25
Joined: Fri Mar 02, 2018 11:04 pm

Re: Post Processor help for Centroid Mill Control

Post by Brian Lamb »

OK, our posts kind of passed each other there. I understand what you mean about the clearance and plunge safety clearance. I left Clearance at Z.1 and changed Safety to Z.05 and it works as it should.

I also unchecked the X and Y boxes in the Parking position and wrote M25 on one line then X16 Y2 on the next and it fixed the order off things at the end.

I'm seeing two M25 codes now, not sure why. I know I had added one to the G40 line at the very beginning of the program, that I can take back out of the post as you now have it showing up before the first tool. Or maybe you have it before and after a tool now? And we need it after and I can use the manually inserted one on the G40 line at the beginning to make sure the quill is up before any movement?

I really appreciate the help... this is already worlds better than it was...
Post Reply