Questions and problems with Sheetcam

Hi Les,

I see that you have been very busy and I hate to bother, but I’m running into some issues that are starting to get under my skin and cause some crashes. This is for a milling machine, so not related to plasma or laser type posts.

First problem, when I post a program, it’s a crap shoot as to wether SC will insert a rapid Z move to R level at the beginning of each tool, sometimes it does, sometimes it doesn’t. Not a huge issue as without it just feeds at the last G01 feedrate all the way down.

Second, when the program calls for a Z depth on the tool, say I’m milling around a contour at Z-.500 (working in inches by the way), the program has a G01 Z-.5 F20 on one line, then followed by XY moves to contour, the problem is it repeats the Z depth on almost every line. This is a big issue, if I decide I only want to go .400 deep, I have to go thru and maybe change 30-50 lines of code, and if I miss just one instance of the Z-.500…. I get a crash… just wiped out a set of expensive hard jaws on my vise yesterday. So… given the Z depth is modal, and there is no need to repeat it line after line unless it changes, can this be edited in the post? Do not post a Z value until it changes?

Third, it also posts a lot of null values, especially I’s and J’s in my G02/03 lines, I was used to if I, J, or K were zero value, you didn’t input them…. this doesn’t effect anything, just something that creates more to look through in the program.

Fourth, I had asked you to help me with using canned drilling cycles and while it kind of works now, it always defaults to G83, peck drilling. Can we define that if the total Z depth and the peck amount are equal it uses G81, spot drilling (or alternately have a check box in SC that lets us define which G-code canned cycle we want)? Then that would leave out the Q value, which is the peck amount, I also found I don’t need a D value. When a canned cycle is called, it also has to have the XY position of the first hole in that line, or it won’t drill, which is what is happening now. Also, if you are drilling just one hole, I use G98 G83 X0 Y0 Z-.5 R.1 Q.25 F10 that has the drill retract to the initial level after the hole. If it is a series of holes, then you need the first line to be G99 G83…… and then you need G98 X_ Y_ on the last line. Also, after the canned cycle has been used, the next line after the last hole has to be G80 to cancel the canned cycle.

I know most folks don’t use canned cycles and just let SC pump out miles of code in place of canned cycles, but there are too many times I find a peck of .35 needs to be changed to .25, if it’s in a canned cycle, it’s one value to change in the code at the machine. If it’s posted “long hand” so to speak, it’s go into the house, pull up SC, modify the parameter for peck amount, re-post, send back to the shop computer, load to machine…. and as luck always has it, it’s a program I had to heavily modify… which means I have to do it all over again.

This kind of falls under niggling, but my comments (tool # such and such, description of the tool) come out quite a few lines above where they should be, could those be put right above the T_ _ call?

I’ll try to attach a program, unedited and then after I have cleaned it up, also the job file.


\

Yahoo Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/sheetcam/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/sheetcam/join
(Yahoo! ID required)

<*> To change settings via email:
sheetcam-digest@yahoogroups.com
sheetcam-fullfeatured@yahoogroups.com

<*> To unsubscribe from this group, send an email to:
sheetcam-unsubscribe@yahoogroups.com

<*> Your use of Yahoo Groups is subject to:
https://info.yahoo.com/legal/us/yahoo/utos/terms/




Brian Lamb
blamb11@cox.net
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”

On Sat, 26 Apr 2014 15:21:38 -0700, you wrote:

First problem, when I post a program, it’s a crap shoot as to wether SC will insert a rapid Z move to R level at the beginning of each tool, sometimes it does, sometimes it doesn’t. Not a huge issue as without it just feeds at the last G01 feedrate all the way down.

Put a G0 in your post processor if you need one

Second, when the program calls for a Z depth on the tool, say I’m milling around a contour at Z-.500 (working in inches by the way), the program has a G01 Z-.5 F20 on one line, then followed by XY moves to contour, the problem is it repeats the Z depth on almost every line. This is a big issue, if I decide I only want to go .400 deep, I have to go thru and maybe change 30-50 lines of code, and if I miss just one instance of the Z-.500…. I get a crash… just wiped out a set of expensive hard jaws on my vise yesterday. So… given the Z depth is modal, and there is no need to repeat it line after line unless it changes, can this be edited in the post? Do not post a Z value until it changes?

Alter then rerun the CAM much safer and quicker. Alternately use an
editor where you can search and replace a word in all or a section only
of the file. Notepad++ is excellent, and free. Available here

http://notepad-plus-plus.org/

Third, it also posts a lot of null values, especially I’s and J’s in my G02/03 lines, I was used to if I, J, or K were zero value, you didn’t input them…. this doesn’t effect anything, just something that creates more to look through in the program.

G2/G3 the I’s and J’s are mandatory, they have to be stipulated even if
they are 0 - its a code error otherwise and controller should stop.

Fourth, I had asked you to help me with using canned drilling cycles and while it kind of works now, it always defaults to G83, peck drilling. Can we define that if the total Z depth and the peck amount are equal it uses G81, spot drilling (or alternately have a check box in SC that lets us define which G-code canned cycle we want)? Then that would leave out the Q value, which is the peck amount, I also found I don’t need a D value. When a canned cycle is called, it also has to have the XY position of the first hole in that line, or it won’t drill, which is what is happening now. Also, if you are drilling just one hole, I use G98 G83 X0 Y0 Z-.5 R.1 Q.25 F10 that has the drill retract to the initial level after the hole. If it is a series of holes, then you need the first line to be G99 G83…… and then you need G98 X_ Y_ on the last line. Also, after the canned cycle has been used, the next line after the last hole has to be G80 to cancel the canned cycle.

You don’t say what control program you are using but if you are using
Mach3 there may well be a bug in the 1083.m1s file. If it’s not dated
August 2005 - it’s buggy. If it mentions John Guenther in the changes
section it’s broken. If not, edit the post processor. If you need the
correct 1083.m1s file - ask.

I know most folks don’t use canned cycles and just let SC pump out miles of code in place of canned cycles, but there are too many times I find a peck of .35 needs to be changed to .25, if it’s in a canned cycle, it’s one value to change in the code at the machine. If it’s posted “long hand” so to speak, it’s go into the house, pull up SC, modify the parameter for peck amount, re-post, send back to the shop computer, load to machine…. and as luck always has it, it’s a program I had to heavily modify… which means I have to do it all over again.

Again - rerun CAM - FAR less chance for an error or put a copy of
sheetcam on the PC in the workshop.

This kind of falls under niggling, but my comments (tool # such and such, description of the tool) come out quite a few lines above where they should be, could those be put right above the T_ _ call?

The comment lines seem to start where that action starts?

Steve Blackmore


\

Yahoo Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/sheetcam/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/sheetcam/join
(Yahoo! ID required)

<*> To change settings via email:
sheetcam-digest@yahoogroups.com
sheetcam-fullfeatured@yahoogroups.com

<*> To unsubscribe from this group, send an email to:
sheetcam-unsubscribe@yahoogroups.com

<*> Your use of Yahoo Groups is subject to:
https://info.yahoo.com/legal/us/yahoo/utos/terms/

Hi Steve,

Thanks for the reply. I was able to spend some hours last night on this and found a couple of posts, Fanuc 6M and Fanuc Mill and tried posting using them instead of my modified Mach 3 post. They did manage to get rid of the redundant Z depth and Feed rate call outs, so I examined the actual post processors and figured out using ### in stead of zeros gets rid of a lot of following zero’s, and changing a few “ModalNumber” to “NonModalNumber” got rid of the extra feedrate calls.


I’m using a Milltronics Centurion V control, uses “normal” g-codes and is probably most similar to a generic Fanuc post… it has some extra g-codes that do some other functions, but Fanuc gets me close. Not sure about your software, but any Fanuc, Fadal, Milltronics, and most other industrial processors that I have run into you don’t need an I, J, or K posted on the G02/03 line if the value is zero. For example a circle on 0,0 would look like this:


G00 X0 Y0
G01 Z-.5 F10
X.25
G03 I-.25
G01 X-.25
G00 Z.1


On my G03 line, I don’t need X and Y as it’s a full circle and I have no change in start to end position. No need for a J value as it is zero.


Using an editor, I do, One CNC has a nice free communications and editing software, called oneDNC or NCLink, think one was earlier than the other, but somehow I have both, like the NCLink one better. I do a lot of editing in that now, but it would be nice to have the post do as close to correct as it can, any manual editing I do is bound to be prone to errors, so less is better.


Likewise, re-posting in the shop isn’t the most productive, I work from a wheelchair and I have my shop computer stuffed into a shelving unit to the right of the machine… use a bluetooth keyboard on my lap, squinting at the monitor… so while it’s adequate for transferring the program back and forth from the machine, it’s a bit frustrating to try to do any real programming or such there. Plus, the whole open the software, modify a value, re-post, then send back to the machine, just to change a depth, a peck, or finish amount on an endmill as it wears is kind of bassackwards in production when you can just change one Z depth, Q amount, or a D value for using G41/42 on a profile pass.


Comments in the program are about 4-5 lines above where the action starts, for example, here is a portion of the unedited program:


N0530 (Operation: Drill, CENTER, T13: 90 degree csk, 0.16 inch Deep)
N0540 G00 Z0.1000
N0550 M09 (Coolant off)
N0560 M05
N0570 G49 Z0
N0580 X-16.0000 Y-5.0000
N0590 (90 degree csk)
N0600 T2 M06 G43 H2
N0610 M07 (Mist coolant on)
N0620 S1500 M03


As you can see, the First comment line is on line 0530, then I have 0540 thru 0580 that deal with the previous tool before I get to line 0590 that actually starts to deal with the tool the comments are about. If I could get the 0530 line to show up just above or below the 0590 line, that would be much more clear.


I am still stumped on my canned cycles, was able to add in the G99 on the first line, think I may even have the G80 showing up after the drilling, got rid of the values I don’t need, like D and V. It would be nice to figure out how to state “if drillz = drillPeck, then post G81” , then this would be close to what I need for G83…. I think… “if drillz > drillPeck, then post G83”. Or maybe it could be just a check box in the drilling portion of Sheetcam as to which canned cycle you want, G73, G81, G82, G83, G85, G86 or G89 and it would have the correct letter values associated with each call… some need peck amounts, some need dwell values.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”


On Apr 27, 2014, at 1:22 AM, Steve Blackmore <steve@pilotltd.net (steve@pilotltd.net)> wrote:

On Sat, 26 Apr 2014 15:21:38 -0700, you wrote:>First problem, when I post a program, it’s a crap shoot as to wether SC will insert a rapid Z move to R level at the beginning of each tool, sometimes it does, sometimes it doesn’t. Not a huge issue as without it just feeds at the last G01 feedrate all the way down.Put a G0 in your post processor if you need one>Second, when the program calls for a Z depth on the tool, say I’m milling around a contour at Z-.500 (working in inches by the way), the program has a G01 Z-.5 F20 on one line, then followed by XY moves to contour, the problem is it repeats the Z depth on almost every line. This is a big issue, if I decide I only want to go .400 deep, I have to go thru and maybe change 30-50 lines of code, and if I miss just one instance of the Z-.500…. I get a crash… just wiped out a set of expensive hard jaws on my vise yesterday. So… given the Z depth is modal, and there is no need to repeat it line after line unless it changes, can this be edited in the post? Do not post a Z value until it changes?Alter then rerun the CAM much safer and quicker. Alternately use aneditor where you can search and replace a word in all or a section onlyof the file. Notepad++ is excellent, and free. Available here> http://notepad-plus-plus.org/> >Third, it also posts a lot of null values, especially I’s and J’s in my G02/03 lines, I was used to if I, J, or K were zero value, you didn’t input them…. this doesn’t effect anything, just something that creates more to look through in the program.G2/G3 the I’s and J’s are mandatory, they have to be stipulated even ifthey are 0 - its a code error otherwise and controller should stop.>Fourth, I had asked you to help me with using canned drilling cycles and while it kind of works now, it always defaults to G83, peck drilling. Can we define that if the total Z depth and the peck amount are equal it uses G81, spot drilling (or alternately have a check box in SC that lets us define which G-code canned cycle we want)? Then that would leave out the Q value, which is the peck amount, I also found I don’t need a D value. When a canned cycle is called, it also has to have the XY position of the first hole in that line, or it won’t drill, which is what is happening now. Also, if you are drilling just one hole, I use G98 G83 X0 Y0 Z-.5 R.1 Q.25 F10 that has the drill retract to the initial level after the hole. If it is a series of holes, then you need the first line to be G99 G83…… and then you need G98 X_ Y_ on the last line. Also, after the canned cycle has been used, the next line after the last hole has to be G80 to cancel the canned cycle.You don’t say what control program you are using but if you are usingMach3 there may well be a bug in the 1083.m1s file. If it’s not datedAugust 2005 - it’s buggy. If it mentions John Guenther in the changessection it’s broken. If not, edit the post processor. If you need thecorrect 1083.m1s file - ask.>I know most folks don’t use canned cycles and just let SC pump out miles of code in place of canned cycles, but there are too many times I find a peck of .35 needs to be changed to .25, if it’s in a canned cycle, it’s one value to change in the code at the machine. If it’s posted “long hand” so to speak, it’s go into the house, pull up SC, modify the parameter for peck amount, re-post, send back to the shop computer, load to machine…. and as luck always has it, it’s a program I had to heavily modify… which means I have to do it all over again.Again - rerun CAM - FAR less chance for an error or put a copy ofsheetcam on the PC in the workshop.>This kind of falls under niggling, but my comments (tool # such and such, description of the tool) come out quite a few lines above where they should be, could those be put right above the T_ _ call?The comment lines seem to start where that action starts?Steve Blackmore–



.,._

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

OK, I spent last night and some more this morning fine tuning posts. I have the post leaving off all the extra feedrates and Z depths now. What I still would like, is to have the “OnNewOperation” line be just above the OnComment line. If possible, could the OnNewOperation line also include the Finish allowance in the comments? A lot of times I do the same profile pass with .200” stock, then .100” then .010” then .000” it would be nice to see that in the comment line.

I have the canned cycle posting G99 and G83 on the first line, the X and Y values in that line every time now. How do I get the last drill position line to have G98 in front of it? I did get the G80 to post after the drill function. Would still be nice to be able to use other canned cycles…… not sure if that would be easier to incorporate into the operation portion of SC rather than the post portion.


I’m using G32 to retract the quill on my knee mill to the tool change position, so added that in as a line above the move to tool change position. That works for all the tools, but at the end of the program, when the machine goes to move to the parking position, I would like to add G32 one line above the move to the parking position, would like to make sure the quill is retracted before the machine takes off in XY. I can’t find any mention of the parking position at all in the post.


So, after a half dozen hours of messing about, I have it pretty close, could just use some help finalizing. I created a support file and uploaded it direct.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”


On Apr 26, 2014, at 3:21 PM, Brian Lamb <blamb11@cox.net (blamb11@cox.net)> wrote:

Hi Les,I see that you have been very busy and I hate to bother, but I’m running into some issues that are starting to get under my skin and cause some crashes. This is for a milling machine, so not related to plasma or laser type posts. First problem, when I post a program, it’s a crap shoot as to wether SC will insert a rapid Z move to R level at the beginning of each tool, sometimes it does, sometimes it doesn’t. Not a huge issue as without it just feeds at the last G01 feedrate all the way down.Second, when the program calls for a Z depth on the tool, say I’m milling around a contour at Z-.500 (working in inches by the way), the program has a G01 Z-.5 F20 on one line, then followed by XY moves to contour, the problem is it repeats the Z depth on almost every line. This is a big issue, if I decide I only want to go .400 deep, I have to go thru and maybe change 30-50 lines of code, and if I miss just one instance of the Z-.500…. I get a crash… just wiped out a set of expensive hard jaws on my vise yesterday. So… given the Z depth is modal, and there is no need to repeat it line after line unless it changes, can this be edited in the post? Do not post a Z value until it changes?Third, it also posts a lot of null values, especially I’s and J’s in my G02/03 lines, I was used to if I, J, or K were zero value, you didn’t input them…. this doesn’t effect anything, just something that creates more to look through in the program.Fourth, I had asked you to help me with using canned drilling cycles and while it kind of works now, it always defaults to G83, peck drilling. Can we define that if the total Z depth and the peck amount are equal it uses G81, spot drilling (or alternately have a check box in SC that lets us define which G-code canned cycle we want)? Then that would leave out the Q value, which is the peck amount, I also found I don’t need a D value. When a canned cycle is called, it also has to have the XY position of the first hole in that line, or it won’t drill, which is what is happening now. Also, if you are drilling just one hole, I use G98 G83 X0 Y0 Z-.5 R.1 Q.25 F10 that has the drill retract to the initial level after the hole. If it is a series of holes, then you need the first line to be G99 G83…… and then you need G98 X_ Y_ on the last line. Also, after the canned cycle has been used, the next line after the last hole has to be G80 to cancel the canned cycle.I know most folks don’t use canned cycles and just let SC pump out miles of code in place of canned cycles, but there are too many times I find a peck of .35 needs to be changed to .25, if it’s in a canned cycle, it’s one value to change in the code at the machine. If it’s posted “long hand” so to speak, it’s go into the house, pull up SC, modify the parameter for peck amount, re-post, send back to the shop computer, load to machine…. and as luck always has it, it’s a program I had to heavily modify… which means I have to do it all over again.This kind of falls under niggling, but my comments (tool # such and such, description of the tool) come out quite a few lines above where they should be, could those be put right above the T_ _ call?I’ll try to attach a program, unedited and then after I have cleaned it up, also the job file.

Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com > click on “rescue dogs”

\



.,._

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

Hi Brian,


OK, I spent last night and some more this morning fine tuning posts. I have the post leaving off all the extra feedrates and Z depths now. What I still would like, is to have the “OnNewOperation” line be just above the OnComment line.

I am afraid there isn’t any way to set the order of these two in the post.

If possible, could the OnNewOperation line also include the Finish allowance in the comments? A lot of times I do the same profile pass with .200” stock, then .100” then .010” then .000” it would be nice to see that in the comment line.

It is possible but awkward to program. How important is it to you?

I have the canned cycle posting G99 and G83 on the first line, the X and Y values in that line every time now. How do I get the last drill position line to have G98 in front of it? I did get the G80 to post after the drill function.

Hmm, that would be difficult. The post doesn’t know which is the last drill until it hits OnDrillEnd() which is too late.

Would still be nice to be able to use other canned cycles…… not sure if that would be easier to incorporate into the operation portion of SC rather than the post portion.

I’m not keen on incorporating this in the operation - the drilling cycles seem to vary quite a bit between different machines. You could get the post to use different cycles depending on the drill depth.

I’m using G32 to retract the quill on my knee mill to the tool change position, so added that in as a line above the move to tool change position. That works for all the tools, but at the end of the program, when the machine goes to move to the parking position, I would like to add G32 one line above the move to the parking position, would like to make sure the quill is retracted before the machine takes off in XY. I can’t find any mention of the parking position at all in the post.

Normally parking is done in job options and the post has no control over that. If you always park you could hard code parking in the post and remove the parking move from job options. Just add the relevant code to OnFinish().

Les


.,._

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

Hi Les,

The order of the comments, hmm… what triggers the comment to begin with, the T call? I guess I’m just baffled why the OnComment line is perfectly placed and we can’t get the OnNewOperation line in the same spot. It’s not the end of the world though, as these lines have no effect on the actual program, they are just for information only.


Same with the Finish allowance, not the end of the world, I thought it was just adding that value to the comments posted in the OnNewOperation line… shows how little I know about the actual programming side of this software.


The G98 on the last drill line, it can’t do an if/then statement? If the next is OnDrillEnd, then prefix the line with G98? As for using the post to determine which canned cycle, given that 90% of the time it’s either G81 or G83, I suppose figuring that out would be good.


The parking issue, you have the ability to use lines of code for the tool change position, could the parking be the same? That’s how I get the G32 in before the move to the tool change position, so if it could be added into the parking position option that would work.


Regardless of what can or can’t be added, I can always modify the program after posting, been doing that since day one anyway. I was just trying to get as close to what works as possible.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”


On Apr 28, 2014, at 5:31 AM, Les Newell <les.newell@fastmail.co.uk (les.newell@fastmail.co.uk)> wrote:

Hi Brian,

OK, I spent last night and some more this morning fine tuning posts. I have the post leaving off all the extra feedrates and Z depths now. What I still would like, is to have the “OnNewOperation” line be just above the OnComment line.

I am afraid there isn’t any way to set the order of these two in the post.

If possible, could the OnNewOperation line also include the Finish allowance in the comments? A lot of times I do the same profile pass with .200” stock, then .100” then .010” then .000” it would be nice to see that in the comment line.

It is possible but awkward to program. How important is it to you?

I have the canned cycle posting G99 and G83 on the first line, the X and Y values in that line every time now. How do I get the last drill position line to have G98 in front of it? I did get the G80 to post after the drill function.

Hmm, that would be difficult. The post doesn’t know which is the last drill until it hits OnDrillEnd() which is too late.

Would still be nice to be able to use other canned cycles…… not sure if that would be easier to incorporate into the operation portion of SC rather than the post portion.

I’m not keen on incorporating this in the operation - the drilling cycles seem to vary quite a bit between different machines. You could get the post to use different cycles depending on the drill depth.

I’m using G32 to retract the quill on my knee mill to the tool change position, so added that in as a line above the move to tool change position. That works for all the tools, but at the end of the program, when the machine goes to move to the parking position, I would like to add G32 one line above the move to the parking position, would like to make sure the quill is retracted before the machine takes off in XY. I can’t find any mention of the parking position at all in the post.

Normally parking is done in job options and the post has no control over that. If you always park you could hard code parking in the post and remove the parking move from job options. Just add the relevant code to OnFinish().Les
\



.,._

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

The comments are taken from the ‘notes’ tab of the tool or operation.

The G98 on the last drill line, it can’t do an if/then statement? If the next is OnDrillEnd, then prefix the line with G98? As for using the post to determine which canned cycle, given that 90% of the time it’s either G81 or G83, I suppose figuring that out would be good.

Unfortunately not. The post does not know what is coming next when it calls OnDrill.

The parking issue, you have the ability to use lines of code for the tool change position, could the parking be the same? That’s how I get the G32 in before the move to the tool change position, so if it could be added into the parking position option that would work.

I need to think on this one. It depends on how useful others would find this.

Les


On 28/04/2014 15:02, Brian Lamb wrote:

Hi Les,

The order of the comments, hmm… what triggers the comment to begin with, the T call? I guess I’m just baffled why the OnComment line is perfectly placed and we can’t get the OnNewOperation line in the same spot. It’s not the end of the world though, as these lines have no effect on the actual program, they are just for information only.


Same with the Finish allowance, not the end of the world, I thought it was just adding that value to the comments posted in the OnNewOperation line… shows how little I know about the actual programming side of this software.


The G98 on the last drill line, it can’t do an if/then statement? If the next is OnDrillEnd, then prefix the line with G98? As for using the post to determine which canned cycle, given that 90% of the time it’s either G81 or G83, I suppose figuring that out would be good.


The parking issue, you have the ability to use lines of code for the tool change position, could the parking be the same? That’s how I get the G32 in before the move to the tool change position, so if it could be added into the parking position option that would work.


Regardless of what can or can’t be added, I can always modify the program after posting, been doing that since day one anyway. I was just trying to get as close to what works as possible.
Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com > click on “rescue dogs”


On Apr 28, 2014, at 5:31 AM, Les Newell <> les.newell@fastmail.co.uk > (> les.newell@fastmail.co.uk> )> wrote:

Hi Brian,

OK, I spent last night and some more this morning fine tuning posts. I have the post leaving off all the extra feedrates and Z depths now. What I still would like, is to have the “OnNewOperation” line be just above the OnComment line.

I am afraid there isn’t any way to set the order of these two in the post.

If possible, could the OnNewOperation line also include the Finish allowance in the comments? A lot of times I do the same profile pass with .200” stock, then .100” then .010” then .000” it would be nice to see that in the comment line.

It is possible but awkward to program. How important is it to you?

I have the canned cycle posting G99 and G83 on the first line, the X and Y values in that line every time now. How do I get the last drill position line to have G98 in front of it? I did get the G80 to post after the drill function.

Hmm, that would be difficult. The post doesn’t know which is the last drill until it hits OnDrillEnd() which is too late.

Would still be nice to be able to use other canned cycles…… not sure if that would be easier to incorporate into the operation portion of SC rather than the post portion.

I’m not keen on incorporating this in the operation - the drilling cycles seem to vary quite a bit between different machines. You could get the post to use different cycles depending on the drill depth.

I’m using G32 to retract the quill on my knee mill to the tool change position, so added that in as a line above the move to tool change position. That works for all the tools, but at the end of the program, when the machine goes to move to the parking position, I would like to add G32 one line above the move to the parking position, would like to make sure the quill is retracted before the machine takes off in XY. I can’t find any mention of the parking position at all in the post.

Normally parking is done in job options and the post has no control over that. If you always park you could hard code parking in the post and remove the parking move from job options. Just add the relevant code to OnFinish(). Les

\

\



.,._

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

I understand the comments come from the notes section, what I meant was what triggers the software to post them in the program? The way the post looks it creates the line based on the function “OnNewOperation” and I’m not understanding why that happens 3 to 6 lines above the tool call. I just had an idea, could the “post.Text (“ (Operation: “, operationName, “)\n) be removed from OnNewOperation and be inserted into the first lines of OnToolChange? Then the comments would be on the line directly above the T01M06G43 H01?

I’ll add in the G98 as needed then.


In regards to adding the G32 or G28 or G49Z0 after the last tool and before moving to an XY parking position, how do other folks with mills do it? Any knee mill you need to retract the quill so you don’t crash into the vise, fixture, whatever. If the machine is a VMC, bedmill, or CNC router with a retracting spindle head, again, you need to go to full height to move the machine, and we always moved the machine to a convenient load/unload position. Even with Plasma machines, don’t folks need to move the carriage down to one end of the machine so you can load/unload the sheet of parts you have just cut?


It would seem necessary or useful to anybody…. unless everybody else is doing things completely different than I do… which could be the case I guess, but if it is, I’d like to know how they get around it.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”


On Apr 28, 2014, at 8:18 AM, Les Newell <les.newell@fastmail.co.uk (les.newell@fastmail.co.uk)> wrote:

The comments are taken from the ‘notes’ tab of the tool or operation.

The G98 on the last drill line, it can’t do an if/then statement? If the next is OnDrillEnd, then prefix the line with G98? As for using the post to determine which canned cycle, given that 90% of the time it’s either G81 or G83, I suppose figuring that out would be good.

Unfortunately not. The post does not know what is coming next when it calls OnDrill.

The parking issue, you have the ability to use lines of code for the tool change position, could the parking be the same? That’s how I get the G32 in before the move to the tool change position, so if it could be added into the parking position option that would work.

I need to think on this one. It depends on how useful others would find this.LesOn 28/04/2014 15:02, Brian Lamb wrote:

Hi Les,
The order of the comments, hmm… what triggers the comment to begin with, the T call? I guess I’m just baffled why the OnComment line is perfectly placed and we can’t get the OnNewOperation line in the same spot. It’s not the end of the world though, as these lines have no effect on the actual program, they are just for information only.

Same with the Finish allowance, not the end of the world, I thought it was just adding that value to the comments posted in the OnNewOperation line… shows how little I know about the actual programming side of this software.

The G98 on the last drill line, it can’t do an if/then statement? If the next is OnDrillEnd, then prefix the line with G98? As for using the post to determine which canned cycle, given that 90% of the time it’s either G81 or G83, I suppose figuring that out would be good.

The parking issue, you have the ability to use lines of code for the tool change position, could the parking be the same? That’s how I get the G32 in before the move to the tool change position, so if it could be added into the parking position option that would work.

Regardless of what can or can’t be added, I can always modify the program after posting, been doing that since day one anyway. I was just trying to get as close to what works as possible.Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com > click on “rescue dogs”

On Apr 28, 2014, at 5:31 AM, Les Newell <> les.newell@fastmail.co.uk > (> les.newell@fastmail.co.uk> )> wrote:

Hi Brian,
I am afraid there isn’t any way to set the order of these two in the post.It is possible but awkward to program. How important is it to you?Hmm, that would be difficult. The post doesn’t know which is the last drill until it hits OnDrillEnd() which is too late.I’m not keen on incorporating this in the operation - the drilling cycles seem to vary quite a bit between different machines. You could get the post to use different cycles depending on the drill depth.Normally parking is done in job options and the post has no control over that. If you always park you could hard code parking in the post and remove the parking move from job options. Just add the relevant code to OnFinish().Les

\



.,._

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

OK, I tested the moving of the comments into the ontoolchange, that worked perfectly, but if I remove the onnewoperation part, I don’t get the comments repeated when I’m using the same tool for a second, third or fourth operation. So, I just left them both in and I’ll delete the extra line that is 4-6 lines too high from the beginning of the tool change.
Brian Lamb
blamb11@cox.net (blamb11@cox.net)
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”


On Apr 28, 2014, at 11:48 AM, Brian Lamb <blamb11@cox.net (blamb11@cox.net)> wrote:

I understand the comments come from the notes section, what I meant was what triggers the software to post them in the program? The way the post looks it creates the line based on the function “OnNewOperation” and I’m not understanding why that happens 3 to 6 lines above the tool call. I just had an idea, could the “post.Text (“ (Operation: “, operationName, “)\n) be removed from OnNewOperation and be inserted into the first lines of OnToolChange? Then the comments would be on the line directly above the T01M06G43 H01?
I’ll add in the G98 as needed then.

In regards to adding the G32 or G28 or G49Z0 after the last tool and before moving to an XY parking position, how do other folks with mills do it? Any knee mill you need to retract the quill so you don’t crash into the vise, fixture, whatever. If the machine is a VMC, bedmill, or CNC router with a retracting spindle head, again, you need to go to full height to move the machine, and we always moved the machine to a convenient load/unload position. Even with Plasma machines, don’t folks need to move the carriage down to one end of the machine so you can load/unload the sheet of parts you have just cut?

It would seem necessary or useful to anybody…. unless everybody else is doing things completely different than I do… which could be the case I guess, but if it is, I’d like to know how they get around it.Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com > click on “rescue dogs”

On Apr 28, 2014, at 8:18 AM, Les Newell <> les.newell@fastmail.co.uk > (> les.newell@fastmail.co.uk> )> wrote:

The comments are taken from the ‘notes’ tab of the tool or operation.

The G98 on the last drill line, it can’t do an if/then statement? If the next is OnDrillEnd, then prefix the line with G98? As for using the post to determine which canned cycle, given that 90% of the time it’s either G81 or G83, I suppose figuring that out would be good.

Unfortunately not. The post does not know what is coming next when it calls OnDrill.

The parking issue, you have the ability to use lines of code for the tool change position, could the parking be the same? That’s how I get the G32 in before the move to the tool change position, so if it could be added into the parking position option that would work.

I need to think on this one. It depends on how useful others would find this.LesOn 28/04/2014 15:02, Brian Lamb wrote:

Hi Les,
The order of the comments, hmm… what triggers the comment to begin with, the T call? I guess I’m just baffled why the OnComment line is perfectly placed and we can’t get the OnNewOperation line in the same spot. It’s not the end of the world though, as these lines have no effect on the actual program, they are just for information only.

Same with the Finish allowance, not the end of the world, I thought it was just adding that value to the comments posted in the OnNewOperation line… shows how little I know about the actual programming side of this software.

The G98 on the last drill line, it can’t do an if/then statement? If the next is OnDrillEnd, then prefix the line with G98? As for using the post to determine which canned cycle, given that 90% of the time it’s either G81 or G83, I suppose figuring that out would be good.

The parking issue, you have the ability to use lines of code for the tool change position, could the parking be the same? That’s how I get the G32 in before the move to the tool change position, so if it could be added into the parking position option that would work.

Regardless of what can or can’t be added, I can always modify the program after posting, been doing that since day one anyway. I was just trying to get as close to what works as possible.Brian Lamb
blamb11@cox.net > (> blamb11@cox.net> )
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com > click on “rescue dogs”

On Apr 28, 2014, at 5:31 AM, Les Newell <> les.newell@fastmail.co.uk > (> les.newell@fastmail.co.uk> )> wrote:

.,._

Visit Your Group

Unsubscribe (<sheetcam-unsubscribe@yahoogroups.com>?subject=Unsubscribe) • Terms of Use



,.,_

Hi Brian,

I understand the comments come from the notes section, what I meant
was what triggers the software to post them in the program?

The operation comments are output just after OnNewOperation.

The way the post looks it creates the line based on the function
“OnNewOperation” and I’m not understanding why that happens 3 to 6
lines above the tool call.

Tool change only happens when SheetCam detects it needs to change a
tool, in other words when it starts a new cut that uses a different tool
to the previous cut.

In regards to adding the G32 or G28 or G49Z0 after the last tool and
before moving to an XY parking position, how do other folks with mills
do it?

I see your point. I’ll look into adding something to get around the problem.

Les

\

Yahoo Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/sheetcam/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/sheetcam/join
(Yahoo! ID required)

<*> To change settings via email:
sheetcam-digest@yahoogroups.com
sheetcam-fullfeatured@yahoogroups.com

<*> To unsubscribe from this group, send an email to:
sheetcam-unsubscribe@yahoogroups.com

<*> Your use of Yahoo Groups is subject to:
https://info.yahoo.com/legal/us/yahoo/utos/terms/

Hi Les,

First, thank you for taking the time to even look at all of this. I played with changing the location of the comments, by moving the comments call to the OnToolChange section I can get the comments exactly where I wanted them, but then I do loose the comments when the tool doesn’t change but the operation does…. like using the same endmill to take a pass at .200” final stock, then .100” and so on. So, leaving the comments call after the OnNewOperation works too and I can just ignore or delete the extra comment lines I get in the program.

My confusion comes from seeing that comment line show up approximately 5 lines from the actual beginning of the new operation…. my comments are before the last tool is rapid back to clearance level, coolant is turned off, spindle stopped, return to tool change level and tool change position. That all seems to be way before the condition of OnNewOperation, see code below:

N3100 G03 X1.9074 Y-2.368 I0 J-0.128
N3110 (Operation: Drill, CENTER, T32: .370 dia. Single point thread mill, 0.025 inch Deep)
N3120 G00 Z0.1
N3130 M09 (Coolant off)
N3140 M05
N3150 G32
N3160 G00 X-4 Y-4
N3170 (.370 dia. Single point thread mill)
N3180 T2 M06 G43 H2

Unfortunately, I think this is a case of just like dealing with a young child…. “but dad, why does it do this”, and you are going to have to tell me “just because dad says so, now go away kid you bother me……” :slight_smile:

Ultimately I am trying to make the software work better for the machining guys, and I suspect 90% of your users are plasma type guys… which makes sense with software named “SheetCam”. So I understand the lack of desire to change for a smaller base of users. I like the ability and simplicity of the software though, and would like to continue to use/develop it to do as good a job as possible.

Brian Lamb
blamb11@cox.net
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com click on “rescue dogs”



On Apr 29, 2014, at 9:28 AM, Les Newell <les.newell@fastmail.co.uk> wrote:

Hi Brian,

I understand the comments come from the notes section, what I meant
was what triggers the software to post them in the program?

The operation comments are output just after OnNewOperation.

The way the post looks it creates the line based on the function
“OnNewOperation” and I’m not understanding why that happens 3 to 6
lines above the tool call.

Tool change only happens when SheetCam detects it needs to change a
tool, in other words when it starts a new cut that uses a different tool
to the previous cut.

In regards to adding the G32 or G28 or G49Z0 after the last tool and
before moving to an XY parking position, how do other folks with mills
do it?

I see your point. I’ll look into adding something to get around the problem.

Les

\

Yahoo Groups Links
\


Yahoo Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/sheetcam/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/sheetcam/join
(Yahoo! ID required)

<*> To change settings via email:
sheetcam-digest@yahoogroups.com
sheetcam-fullfeatured@yahoogroups.com

<*> To unsubscribe from this group, send an email to:
sheetcam-unsubscribe@yahoogroups.com

<*> Your use of Yahoo Groups is subject to:
https://info.yahoo.com/legal/us/yahoo/utos/terms/

Hi Brian,

My confusion comes from seeing that comment line show up approximately 5 lines from the actual beginning of the new operation…. my comments are before the last tool is rapid back to clearance level, coolant is turned off, spindle stopped, return to tool change level and tool change position.

The moves to safe height etc only occur when they are needed. SheetCam
starts a new operation then works out what it needs to do to run that
operation.

Try this:
function OnPenDown()
if commentText then
post.Text(" (“,commentText,”)\n")
commentText = nil
end
end

This will put the comments just before the first plunge of the operation.

By the way if you really want to show the finish allowance you can use
this code:

local part = sc.Parts:Get():op_index(partIndex)
if part then
local op = part.operations:op_index(operationIndex)
if op then
val = op:GetValue(“Finish allowance”)
if val then
post.Text(" (finish allowance: ", val:GetValueString() ,
“)\n”)
end
end
end


Ultimately I am trying to make the software work better for the machining guys, and I suspect 90% of your users are plasma type guys… which makes sense with software named “SheetCam”. So I understand the lack of desire to change for a smaller base of users. I like the ability and simplicity of the software though, and would like to continue to use/develop it to do as good a job as possible.

SheetCam was originally aimed towards wood machining, especially panel
work. The plasma side just evolved somehow. The main reason why I
dislike making changes is that I need to keep it simple. The more
features I add the more likley people are to get confused and have
problems.

In the case of parking I see your point and I think it is worth adding.

Les

On 29/04/2014 18:17, Brian Lamb wrote:

Hi Les,

First, thank you for taking the time to even look at all of this. I played with changing the location of the comments, by moving the comments call to the OnToolChange section I can get the comments exactly where I wanted them, but then I do loose the comments when the tool doesn’t change but the operation does…. like using the same endmill to take a pass at .200” final stock, then .100” and so on. So, leaving the comments call after the OnNewOperation works too and I can just ignore or delete the extra comment lines I get in the program.

My confusion comes from seeing that comment line show up approximately 5 lines from the actual beginning of the new operation…. my comments are before the last tool is rapid back to clearance level, coolant is turned off, spindle stopped, return to tool change level and tool change position. That all seems to be way before the condition of OnNewOperation, see code below:

N3100 G03 X1.9074 Y-2.368 I0 J-0.128
N3110 (Operation: Drill, CENTER, T32: .370 dia. Single point thread mill, 0.025 inch Deep)
N3120 G00 Z0.1
N3130 M09 (Coolant off)
N3140 M05
N3150 G32
N3160 G00 X-4 Y-4
N3170 (.370 dia. Single point thread mill)
N3180 T2 M06 G43 H2

Unfortunately, I think this is a case of just like dealing with a young child…. “but dad, why does it do this”, and you are going to have to tell me “just because dad says so, now go away kid you bother me……” > :slight_smile:

Ultimately I am trying to make the software work better for the machining guys, and I suspect 90% of your users are plasma type guys… which makes sense with software named “SheetCam”. So I understand the lack of desire to change for a smaller base of users. I like the ability and simplicity of the software though, and would like to continue to use/develop it to do as good a job as possible.

Brian Lamb
blamb11@cox.net
Weimaraner Rescue of Arizona
www.vswc.weimaraner.com > click on “rescue dogs”


Yahoo Groups Links

<*> To visit your group on the web, go to:
http://groups.yahoo.com/group/sheetcam/

<*> Your email settings:
Individual Email | Traditional

<*> To change settings online go to:
http://groups.yahoo.com/group/sheetcam/join
(Yahoo! ID required)

<*> To change settings via email:
sheetcam-digest@yahoogroups.com
sheetcam-fullfeatured@yahoogroups.com

<*> To unsubscribe from this group, send an email to:
sheetcam-unsubscribe@yahoogroups.com

<*> Your use of Yahoo Groups is subject to:
https://info.yahoo.com/legal/us/yahoo/utos/terms/