-
Postprocessor questions...
I'll probably have a few post processor questions so I'll use this topic to keep them all in one place and document my customizations.
I'm running a Grizzly G0704 mill converted to CNC with travels: X = 19", Y = 9", Z = 12" using Mach3 as the controller.
In looking at the BC supplied posts (for a Mach3 controller) I see a block at the start:
(BEGIN PREDATOR NC HEADER)
(MCH_FILE=4AXVMILL.MCH)
(MTOOL T5 S1 D.1875 H2. A0. C0. DIAM_OFFSET 5 = .0938)
(SBOX X-2.125 Y-2.125 Z-.125 L4.25 W4.25 H.125)
(END PREDATOR NC HEADER)
I understand that Predator is a gcode editor and back plotter. I use GWizardE from CNCCookbook so I don't really use Predator (and I don't think I have a license for the back plot capability). So, the question is, is there any harm with removing the predator header? I would think not.
I saw on the BC forum that someone asked about launching GWizardE instead of Predator last year. Seemed that there was an issue with GWizardE at the time. Not sure if it's been fixed yet. Does anyone know? If not, I'll take a look.
cheers,
Michael
-
Re: Postprocessor questions...
It doesn`t matter whether you leave it in or not, it is all in (brackets) so will be ignored by Mach3 anyway as Mach3 will see it as comments.
In my experience the Predator Editor with the Backplot is second to none, it has full solid simulation and you can create STL files for your vise, machine bed, clamps etc, etc, means you can see exactly what will be cut and where in solids, I definitely wouldn`t be wouldn`t be without it, best tool in the box for sure and I`m sure you will hear this echoed by others who have it ! !
Also includes your DNC for uploading files to the machine, not of great use with Mach3 as pretty much all of the PC hard drive is available for loading programs to so memory space isn`t an issue.
For those who need to "drip feed" to a machine control with limited memory then it is a great tool.
IMHO for what it`s worth if you are thinking of spending any money on an Editor/Backplotter then I would say seriously consider asking what you can get your Predator upgraded for ! ! !
- - - Updated - - -
-
Re: Postprocessor questions...
Thanks. I already own GWizardE and just used to it. When I moved to BobCAD-CAM I wasn't expecting to change my entire workflow :)
I do see that it is commented, it's just that I read the comments when I load into Mach and like to have the stock size and tool list along with version # up top. Easy changes.
- - - Updated - - -
Thanks. I already own GWizardE and just used to it. When I moved to BobCAD-CAM I wasn't expecting to change my entire workflow :)
I do see that it is commented, it's just that I read the comments when I load into Mach and like to have the stock size and tool list along with version # up top. Easy changes.
-
Re: Postprocessor questions...
Double threads,double posts,what's going on ?????????
I am "Echoing" Engine Guy, pay the coin and get Preditor. level 2 or 3.You should be able to haggle a good deal.Ain't that much,especially for piece of mind.It is proven to run seamlessly with BoB.
- - - Updated - - -
-
Re: Postprocessor questions...
What happened is when I posted the original, I got a system error page from CNCZone. I did a back browse to recover my original post. That had the side effect of making a second post! Sorry about that. There does not appear to be a way for the OP to delete their own post.
Here's what I got:
Invalid headers (404) on line 177 in /home/cnczone/public_html/forums/includes/bitly.php
#0 /home/cnczone/public_html/forums/includes/bitly.php(382): Bitly->doCall('shorten', Array)
#1 /home/cnczone/public_html/forums/newreply.php(937) : eval()'d code(40): Bitly->shorten('http://www.cncz...')
#2 /home/cnczone/public_html/forums/newreply.php(937): eval()
#3 /home/cnczone/public_html/forums/dbseo.php(459): require('/home/cnczone/p...')
#4 {main}
and I got it when I posted this post.
I'll check with my sales guy re: Preditor.
thanks,
Michael
-
Re: Postprocessor questions...
Quote:
Originally Posted by
mhackney
So, the question is, is there any harm with removing the predator header? I would think not.
There wont be any harm or matter to you.
"I" use predator and a lot of the bc users that will help you along use it. If you strip it all out, it will make it harder for me to help, in that the code you are producing wont fit into my workflow for backplotting etc....
An answer of "works fine over here" is not much help to you.....
Those that want to bare bones strip their post and be "minimalists", don't usually need help either.....
-
Re: Postprocessor questions...
Thanks BurrMan. I wouldn't call myself a minimalist. I didn't understand the connection of BobCAM's gcode files to Preditor was made through the predator header, but I understand that now. It looks like the predator header just specifies the machine, the stock dimensions and the tools used. I suppose the back plotter uses that to set the configuration. I have a custom mill defined in BC but the BC provided Mach3 posts have a machine type hardcoded: "(MACH_FILE=HAAS - 3XVMILL.MCH)"
How does Preditor use this? Since I have a home-brew mill, would I have to create a cusomte .MCH for my machine to really leverage Preditor?
I downloaded the limited time trial but its for the previous v9 release. There were a few warts installing and launching but I worked through those. It's a bit pricy - there is only one version offered by BobCAD now - but more importantly, I already have a reasonably sized learning curve with BobCAD-CAM so throwing another application into the mix multiples the pain! Uninstalling Preditor v9 corrupted my v7 that came with BC so I need to reinstall it now.
Cheers,
Michael
-
Re: Postprocessor questions...
Firstly, is anyone else getting the system error page I posted above when you post? I am getting it with every post and it looks like the posts get an "updated" section with the same post repeated! I edited the one above to remove it, I'll leave this one as is so you can see what happens.
I'm still tweaking my Mach3 post to get workable output. I have 1000s of gcode files I created in several other CAM apps with posts that I edited. Nothing fancy but I do a few things fairly routinely and like my code to work a certain way. For instance, my fixtures hold 12 parts. Imagine that these will be 3" diameter donuts cut in 1/8" aluminum with a 2" hole. I cut all the holes first then stop and move the spindle out of the way so I can install circular hold downs so I can mill the perimeters without needing tabs. Usually, a tool change is not made between cutting the holes and perimeter so I need a way to "trigger" stopping the spindle and moving it. BobCAD support answered the first part of the question for me yesterday - I can use multiple machine setups (2 in my case). The post inserts an M00 after the first operation. Now I'm trying to figure out how I can move the spindle, say, to X=Y=0, Z=6 so it's out of the way for me to add the hold downs.
I've read the milling post docs in the post folder. Is there a reference to what all the numbered items are in the file? I'd like to know what a few things are like:
512. Use block delete for stop codes (M00)? n
518. Output M00 codes? n
In particular, 518 - how am I getting the M00 output into my gcode when this seems to say that M00 should not be output!
regards,
Michael
- - - Updated - - -
Firstly, is anyone else getting the system error page I posted above when you post? I am getting it with every post and it looks like the posts get an "updated" section with the same post repeated! I edited the one above to remove it, I'll leave this one as is so you can see what happens.
I'm still tweaking my Mach3 post to get workable output. I have 1000s of gcode files I created in several other CAM apps with posts that I edited. Nothing fancy but I do a few things fairly routinely and like my code to work a certain way. For instance, my fixtures hold 12 parts. Imagine that these will be 3" diameter donuts cut in 1/8" aluminum with a 2" hole. I cut all the holes first then stop and move the spindle out of the way so I can install circular hold downs so I can mill the perimeters without needing tabs. Usually, a tool change is not made between cutting the holes and perimeter so I need a way to "trigger" stopping the spindle and moving it. BobCAD support answered the first part of the question for me yesterday - I can use multiple machine setups (2 in my case). The post inserts an M00 after the first operation. Now I'm trying to figure out how I can move the spindle, say, to X=Y=0, Z=6 so it's out of the way for me to add the hold downs.
I've read the milling post docs in the post folder. Is there a reference to what all the numbered items are in the file? I'd like to know what a few things are like:
512. Use block delete for stop codes (M00)? n
518. Output M00 codes? n
In particular, 518 - how am I getting the M00 output into my gcode when this seems to say that M00 should not be output!
regards,
Michael
-
Re: Postprocessor questions...
The machine filename passed in the post processor is not really processed.. It's more of a marker.. (I think it may tie into "if you have the full blown predator stuff" instead of bc tied in)
The machine file in predator does play a role in how the gcode and stuff is processed though.. But the bc predator is not a "full machine simulator".. That would be the predator virtual cnc level 3, with bc.. They also have full blown standalone versions....
You are correct that the power for predator lies in that header with stock, fixturing, tooling info... The selection of a machine file (done in predator. the listing in the header wont pre-select anything) will have your gcode handled differently per a reverse post processor file that attached to a machine file...
So:
Quote:
How does Preditor use this? Since I have a home-brew mill, would I have to create a cusomte .MCH for my machine to really leverage Preditor?
Predator has a selection for a machine file. This file has some basic info, and is tied to a specific "reverse post processor"... There are some prefabed rvp and machine files that will handle predator with BobCad because it's just a "light version" of the real thing... If you were to go full blown, then all of that stuff would need to be setup per your specific machine.. It's similar to "simulation" regular, vs. simulation pro, with all my machine components... But more "complex" because of the backploting needing to reverse the posting process accurately...
-
Re: Postprocessor questions...
Firstly, thank you for the excellent description.
I see that predator has many components. The editor and virtual cnc seem to be the "right" combo. I wonder if the BC upgrade includes both of those. I don't know what predator component list prices are since they are not listed on the web site.
This is a naive question - what is the difference between BC's simulator and Preditors ritual CNC? I mean, conceptually what's the difference? Couldn't either be used to test for potential problems, collisions, etc? The price I was quoted for the simulator was about the same as for predator (presuming that includes the virtual cmc).
Cheers,
Michael
-
Re: Postprocessor questions...
BobCads new simulation is a "machine simulation" which replaces the old Virtual cnc by predator... 2 different companies. I would stick with BobCads new machine simulation. One benefit is it's is produced by the same people who produce some of the toolpath strategies we are using now..
The only difference is we haven't got "nc code backplot" with the new moduleworks system (But I would guess it's on the radar...) This is what we're still using predator for...
I don't know if they still resale virtual cnc or not (I would guess no), but, that would be the only reason to go that route (The combination of full machine virtualization couple with the backplot of code)... Going that route with predator I think will run past 5K, and would be more of a 3rd party purchase...
BobCads new simulation = "regular" gets you toolpath and stock removal with tool.. Pro gets you your machine visualized in the process...
Backplot is still another added tool, of your choice. Going with predator, it's an "integrated into the workflow" component....
-
Re: Postprocessor questions...
I know you have CNC experience,BUT
Here is my "personal" opinion.If you are a small shop(like just you),Just go with the simulation that comes with BoB.
Reason being,IMO,,,,you got better things to do with your time and money than "playing" with a simulator.Do your CAD,then do your tool paths(CAM),,run it thru Preditor level 2,,,then if you want run the simulation thru the standard version that comes with BoB.
You got a whole new CAM software to learn,IMO learn that,,make chips,collect money.Get a couple years experience with BoB,then decide if you want the fancy simulation.Again,IMO,,spend your time learning the CAD/CAM,,it is what will make parts.
I will add the Preditor is nicely integrated with BoB,meaning it works as though it was made for BoB,in a way.It has paid for itself many times by carefully watching the backplot.CRASHES is what I am talking about.
-
Re: Postprocessor questions...
Thanks guys. jrmach - I see that you must have had the system error - your post is doubled up!
Yes, I'm a 1 guy shop. And I completely agree - I have enough to do as it is! I did need a lathe CAM since I am just bringing my lathe online as CNC. I also did want to move into a more capable mill CNC package - especially with 3D capability. Things worked out and I was able to make the jump with BobCAD-CAM. But now I have the fun of a learning curve and some minor development work to integrate it into my workflow. But, it's been painless so far and I can see where I will have some big gains with time savings and fewer defects.
All that said, I am always listening and learning from those with more or different experiences. I keep and integrate what works for me and my business and cull out that which doesn't. I may be an old dog but I can learn new tricks!
Cheers,
Michael
- - - Updated - - -
Thanks guys. jrmach - I see that you must have had the system error - your post is doubled up!
Yes, I'm a 1 guy shop. And I completely agree - I have enough to do as it is! I did need a lathe CAM since I am just bringing my lathe online as CNC. I also did want to move into a more capable mill CNC package - especially with 3D capability. Things worked out and I was able to make the jump with BobCAD-CAM. But now I have the fun of a learning curve and some minor development work to integrate it into my workflow. But, it's been painless so far and I can see where I will have some big gains with time savings and fewer defects.
All that said, I am always listening and learning from those with more or different experiences. I keep and integrate what works for me and my business and cull out that which doesn't. I may be an old dog but I can learn new tricks!
Cheers,
Michael
-
Re: Postprocessor questions...
Wear many different hats in a one man shop.
-
Re: Postprocessor questions...
That's part of the fun! Except for the "clean the bathroom hat" :(
regards,
Michael
- - - Updated - - -
That's part of the fun! Except for the "clean the bathroom hat" :(
regards,
Michael
-
Re: Postprocessor questions...
I seem to be one of the few who didn't care much for Predator.
The nice thing with using the built in simulation is that you can still have many different machines, and the post is not generated until after you have selected the machine you want to cut it on (bringing up the appropriate post processor automatically). You can change between virtual machines in seconds without having to post out the G-code first. I find this to be a very important distinction because if you post out the G-code, and it's not working well, it's very easy to end up accidentally using a program that you had already decided didn't work right by accident, simply because it exists and you must delete it or update it before you move on in your workflow. If the G-code has not been generated but can be brought right into simulation, there is no opportunity to accidentally use the bad G-code because it does not yet exist.
With the built in Bobcad Standard or Pro simulation system, the last step should be saving the G-code, done only after you have verified that it simulates 100% correctly. This reduces the opportunity to mishandle G-code files that may or may not be kosher for the machine to produce the desired result. In my opinion, having this workflow greatly reduces the option for human error in file handling, which is no small probability for those like me who are probably using half a dozen or more different jump drives to transport the files from their desktop to their CNC machine. Once a file has passed the simulation step, then (and only then) I save it as G-code directly to a jump drive. The only place I save G-code to anymore is the jump drive, and every month or so, I wipe the jump drives clean of all G-code files.
I no longer save G-code files in an archive at all. Let's say that during the year after the initial run of a part from G-code I make changes to the machine, or I buy a second new machine, the only way to know for sure that it will work properly a year later is to re-post it after re-simulating it from the .BBCD file. Any update I make to the machine or post processor would show any problems that there may be, and they would also adjust the G-code output to reflect those changes so the file works correctly. Since the .BBCD file already has the toolpath strategies ready to go, it only takes a few moments to re-verify that the toolpath simulates correctly and post it to G-code. I know that sometimes .BBCD files don't open 100% properly in future versions of Bobcad, but I plan to just keep any older version on hand and keep the post processor and simulation up to date. So far, it seems that both of those are portable, meaning that I can update on version and then put the same machine/post processor files into the other versions, so you really only have to do it once to cover the same update to several versions.
All in all, I really find the Bobcad/Module Works simulator is much more desirable for my own workflow, where Predator never really seemed to fit in well at all. Obviously, there are many who seem to really like it here in the forums, and I imagine they must have a workflow that accommodates it better.
-
Re: Postprocessor questions...
Well, I have gotten myself into a pickle now! I uninstalled the predator v9 demo and now the built in creditor fails in launching. I get a dialog with an error message. I filed a support ticket but the remedy did not work. I completely uninstalled all predator and made sure the registry was clean with Revo and then ran installer to do a repair. Did this twice with no glory.
So rather than fight this, I'd like to send the post to either notepad or my GWizardE editor. I found a post on the BC forum with some VB script on how to launch notepad when you post. But it doesn't work, i.e. nothing happens. I don't know if it is my problem, V27 or maybe a Windows 7 thing. Anyone have any examples of doing something with a visible result using VB script in the post?
thanks,
Michael
-
1 Attachment(s)
Re: Postprocessor questions...
Make sure you are uninstalling everything...look here for preditor
also search forum for this problem.I am thinking versions back to V23 would all be useful information as long as it is 64 bit
and what is the error message say ?
-
Re: Postprocessor questions...
Thanks, I have checked everything for any remnant of predator and there is none. The error is "THREED32.OCX is missing" or something like that.
-
Re: Postprocessor questions...
Quote:
Originally Posted by
mmoe
I seem to be one of the few who didn't care much for Predator.
All in all, I really find the Bobcad/Module Works simulator is much more desirable for my own workflow, where Predator never really seemed to fit in well at all. Obviously, there are many who seem to really like it here in the forums, and I imagine they must have a workflow that accommodates it better.
Hi mmoe,
It didn't appear you made a critical distinction about the 2 tools....
The simulation will verify the "movelist" created by your toolpath features. Essentially, the toolpath you see in the window..... It is not using or looking at any type of gcode....
When you "post your gcode", the process "MillingPostExe.exe" takes your movelist and flavours it per the selected post processor......
It is good to have the ability to verify the gcode as well.....
-
Re: Postprocessor questions...
Quote:
Originally Posted by
mmoe
I seem to be one of the few who didn't care much for Predator.
The nice thing with using the built in simulation is that you can still have many different machines, and the post is not generated until after you have selected the machine you want to cut it on (bringing up the appropriate post processor automatically). You can change between virtual machines in seconds without having to post out the G-code first. I find this to be a very important distinction because if you post out the G-code, and it's not working well, it's very easy to end up accidentally using a program that you had already decided didn't work right by accident, simply because it exists and you must delete it or update it before you move on in your workflow. If the G-code has not been generated but can be brought right into simulation, there is no opportunity to accidentally use the bad G-code because it does not yet exist.
The G code is not brought into the Moduleworks simulation within BobCAD, that runs from the Move List produced, not the G code, it is pretty accurate but not 100%.
What runs OK in the simulation may not be the same in the G code, all depends on how well the PP being used has been setup.
Quote:
Originally Posted by
mmoe
With the built in Bobcad Standard or Pro simulation system, the last step should be saving the G-code, done only after you have verified that it simulates 100% correctly. This reduces the opportunity to mishandle G-code files that may or may not be kosher for the machine to produce the desired result. In my opinion, having this workflow greatly reduces the option for human error in file handling, which is no small probability for those like me who are probably using half a dozen or more different jump drives to transport the files from their desktop to their CNC machine. Once a file has passed the simulation step, then (and only then) I save it as G-code directly to a jump drive. The only place I save G-code to anymore is the jump drive, and every month or so, I wipe the jump drives clean of all G-code files.
Using Predator Backplot doesn`t interfere in any way with your workflow, it only comes into play right at the very end as a final confirmation of the G code, after you have done your simulation and then generated the code that`s where Predator comes into it`s own, simply right click and choose "Edit CNC" and that will launch Predator directly from BobCAD in just the same way that choosing the "Simulation" button in BobCAD launches the Moduleworks simulation, no difference :D
Quote:
Originally Posted by
mmoe
I no longer save G-code files in an archive at all. Let's say that during the year after the initial run of a part from G-code I make changes to the machine, or I buy a second new machine, the only way to know for sure that it will work properly a year later is to re-post it after re-simulating it from the .BBCD file. Any update I make to the machine or post processor would show any problems that there may be, and they would also adjust the G-code output to reflect those changes so the file works correctly. Since the .BBCD file already has the toolpath strategies ready to go, it only takes a few moments to re-verify that the toolpath simulates correctly and post it to G-code. I know that sometimes .BBCD files don't open 100% properly in future versions of Bobcad, but I plan to just keep any older version on hand and keep the post processor and simulation up to date. So far, it seems that both of those are portable, meaning that I can update on version and then put the same machine/post processor files into the other versions, so you really only have to do it once to cover the same update to several versions.
All in all, I really find the Bobcad/Module Works simulator is much more desirable for my own workflow, where Predator never really seemed to fit in well at all. Obviously, there are many who seem to really like it here in the forums, and I imagine they must have a workflow that accommodates it better.
I think everyone does pretty much as you do above, just the added final checking of the actual G code in Predator which can`t currently be done in the Simulator, I do hope that Burr is right in thinking that a proper backplot facility may be added to the software, hopefully sooner rather than later as it is a must as far as I`m concerned :D :D :D
Regards
Rob
:rainfro: :rainfro: :rainfro:
-
Re: Postprocessor questions...
Does anyone have a simple example of a VB script in a post getting called? I tried this:
2101. Read entire file after post.
Dim I As Integer
For I = 1 To 100 ' Loop 100 times.
Beep ' Sound a tone.
Next I
which is as simple as it gets. Nothing happens. I can't find any documentation on how to use the program blocks 2001-2099. A simple beep or popup a modal dialog to validate that I have the plumbing working would be very helpful!
Cheers,
Michael
-
Re: Postprocessor questions...
Ok, digging through the Help and docs in posts/mill/documents I put together what should be the simplest test case to call a script and it is still failing. Here is what I did in my post:
FIRST: I added the line to print a line number, a G and then call the program_block_1:
15. First Machine Setup
" "
"(====================================)"
"(YYY Machine Setup - ",setup_name,")"
"(====================================)"
n,"G",program_block_1
" "
SECOND: I create the simplest script I could for program_block_1:
2001. Program Block 1.
Dim dOffset
dOffset = 28
Mill_SetReturnString(dOffset&)
When I run the post, I see this as output:
(====================================)
(YYY Machine Setup - Hole)
(====================================)
N10 G
I expected to see:
(====================================)
(YYY Machine Setup - Hole)
(====================================)
N10 G28
The script should simply return "28"
So, am I doing something wrong? I can't find a single script that I can verify works in my post on V27 and Windows 7. Is this a V27 bug? Does anyone have a post that successfully executes a (preferable simple) script?
-
1 Attachment(s)
Re: Postprocessor questions...
Let's start simple. Just try this post for starters and see if it does something.
-
1 Attachment(s)
Re: Postprocessor questions...
I'm going to assume that it did do something.
Now edit the post and remove the "carriage returns" and Line 2102. until the blinking cursor is in the same position as it is in this picture:
Attachment 251884
Save it, then post again. You'll notice it quit working. The Scripting engine is a bit picky about how things are organized or laid out. I allow at least two carriage returns between my scripting blocks and at least two at the end of the entire post. The same is true for creating Advanced Posting pages. It just needs it for some reason.
-
Re: Postprocessor questions...
Quote:
Originally Posted by
mhackney
FIRST: I added the line to print a line number, a G and then call the program_block_1:
15. First Machine Setup
" "
"(====================================)"
"(YYY Machine Setup - ",setup_name,")"
"(====================================)"
n,"G",program_block_1
" "
SECOND: I create the simplest script I could for program_block_1:
2001. Program Block 1.
Dim dOffset
dOffset = 28
Mill_SetReturnString(dOffset&)
Your script works fine when I plug it into the post processor I just uploaded. Again, that's with a few carriage returns between the posting blocks. I think you got the gist of it already, you just need to pick up on the little nuances that you will only learn through some testing.
-
Re: Postprocessor questions...
Wow, I don't know what to think about this...
Here's what I did - I took a clean copy of one of the BobCAD posts and added the code above "just to test". Guess what? It worked fine. So I started copying and pasting from my post into this one to look for the culprit code. I was able to copy everything from the header down and the post script continued to work fine. So then I attempted to update the header and all of a sudden the script stopped working. I have a completely reproducible test case that looks like this:
Original header:
---------------------------------------------------------------------
---------------------------------------------------------------------
--- BobCAD-CAM Post Processor --------------------------------------
---------------------------------------------------------------------
--- Initial Software Version: BobCAD-CAM V27
--- Initial Creation Date: x-xx-xxxx
--- Author: BCC
--- Machine: BC_3x_Mill - Optional Stop at Tool Change
---------------------------------------------------------------------
---------------------------------------------------------------------
--- REVISION LOG ----------------------------------------------------
---
--- 10-21-2013 - ACC - Updated end of file to correctly support
--- sub program file end.
--- 5/28/2014 - Initial Setup for V4
--- 8/18/2014 - ACC - Setup for V27
---
---------------------------------------------------------------------
---------------------------------------------------------------------
--- SPECIAL NOTES ABOUT THIS POST AND MACHINE -----------------------
---------------------------------------------------------------------
---
---
---------------------------------------------------------------------
****Version number MONTH DAY YEAR****
1000. Version Information = Version Month Day Year? "10.0 08 18 2014"
If I change the version number from 10.0 to 1.0 the scripts stop running! I can change the date and even add an extra '0' after the decimal like this:
1000. Version Information = Version Month Day Year? "10.00 10 03 2014"
and it works. I can make the 10.0 into 11.0 or 10.1 or 10.00 and these all work, but 1.0 or 1.00 or 01.00 do NOT work! Very very odd behavior.
-
Re: Postprocessor questions...
Quote:
Originally Posted by
mhackney
****Version number MONTH DAY YEAR****
1000. Version Information = Version Month Day Year? "10.0 08 18 2014"
If I change the version number from 10.0 to 1.0 the scripts stop running! I can change the date and even add an extra '0' after the decimal like this:
1000. Version Information = Version Month Day Year? "10.00 10 03 2014"
and it works. I can make the 10.0 into 11.0 or 10.1 or 10.00 and these all work, but 1.0 or 1.00 or 01.00 do NOT work! Very very odd behavior.
That is expected (though unexplained) behavior. At the time scripting was introduced, the post version needed to be at least 9.1 for it to work.
-
Re: Postprocessor questions...
LOL!!!
I thought the Version was MY version for the post. So, since I created my own post, I figured I would start with version 1. No way of knowing that this was used this way. Thanks!
regards,
Michael
-
Re: Postprocessor questions...
Ok, scripting works perfectly now to launch GWizardE with my post. I do have to have file type mapping of .nc to GWizardE as GWE will not launch with a file path. Here's the script:
Code:
2101. Read entire file after post.
'Gather the file name/path
Dim BCC_FILE
BCC_FILE = MILL_GetProgramName()
Sub Run(ByVal sFile)
Dim shell
Set shell = CreateObject("WScript.Shell")
shell.Run Chr(34) & sFile & Chr(34), 1, false
Set shell = Nothing
End Sub
' Execute the program notepad.exe and open BCC_FILE
Run BCC_FILE
Very simple and effective. I tested it both with Post and Post & Save As
Cheers,
Michael
-
Re: Postprocessor questions...
Quote:
Originally Posted by
mhackney
LOL!!!
I thought the Version was MY version for the post. So, since I created my own post, I figured I would start with version 1. No way of knowing that this was used this way. Thanks!
regards,
Michael
LOL, exactly. It's the little things that make scripting hard. The documentation has come a long way but some explanation of those kinds of things would be nice.
-
Re: Postprocessor questions...
mhackney,,,
Preditor Editor just saved me from scrapping a 1/2 days work.A thing called "dog-leg rapids" happens every now and then.The tool path looks perfect,the simulation beautiful,Preditor Editor BAM!!!Can't swear it works for all machines,but you can set it up for Haas.This happened with High Speed Pocketing V 23 AND Advanced Rough V 26 today on a part I was programming...There is no way you would ever of caught it,,not even dry run,I got files on both and will provide on request.Can't emphasize enough how much time and grief Preditor version 2 backplotting has saved me over the years.
BTW,thanks again to SBC for showing me how to set up Preditor for dog legs for Haas.