[redford1955]

we are currently machining small aluminum wings with a 3d airfoil surface. we machine a single wing on a fixture in the middle of the table. production is increasing and we have the need to do 4 wings on a new fixture, but to fit within travels it is necessary to rotate the parts 90 degrees and translate to four positions. we have changed the program from a standard bobcad post to address some of the errors that were present. i need to copy the g code exactly as we are using it, just with different zero and xy coordinates.

thank you
keith

[Force]

G53-G54-G55-G56

[TonyW]

Couple ways to do this. As force says, use the different offsets and just create multiple features. OR, on V25 create multiple machine setups, assign each setup a coordinate system, (G54, 55, 56, 57). Save all your features from the single wing, then load each feature for each machine setup. This way you will only have the one drawing on screen to have to deal with. Since the last update, they fixed the coordinate systems for each machine setup and they seem to work correctly now. Code is posted with each coordinate system value. But verify it with your post, it may need tweaking for either method you use. I've done the multiple machine setup and just label each setup, vise 1, vise 2, etc, or whatever you want to name them.

[bobcad guy]

I assume from what you said, that your program doesn't match whats in the bobcad file, so if you use bob, to try to output 4 wings, they will all have issues, but also you said needing to rotate part 90 degrees. yasnac controls actually have a rotation built in, so if you have yasnac, you can put the program as is, and enter a rotation angle of 90 in the offset page. some fanuc controls use a g67, g68 to allow rotation also. besides that, its back to the bobcad "work around" derby

[BurrMan]

besides that, its back to the bobcad "work around" derby

Thats too bad that you think that setting up BobCad to work properly is a "workaround".... Thats really going to hamper your use of the program, and your ability to run it well......

[bobcad guy]

hey, I agree he should keep the files in bobcad edited to whats in the machine, but sometimes, that just isn't possible. lets take thread milling for instance. I have to manually add cutter comp to the file after bob posts the program, because it will not output a comp to threadmill, atleast not so far in my programs, ive done several threadmill jobs, and will be doing more. I am not going to run back and forth, trying to find out the right number that works, the easiest "workaround" I found is, just add the comp lines after I post it. but how am I supposed to update the program to something it doesn't even support? if you know, please share.

[BurrMan]

Thats too bad that you think that setting up BobCad to work properly is a "workaround".... Thats really going to hamper your use of the program, and your ability to run it well......

Worth a repeat................

[aldepoalo]

with the advance posting tab you can add check boxes pull downs and input fields. you can use for almost anything you want to post. like adding comp

[RAF.]

Al
Maybe you can make a demo or is there already one out ?
Thanks

[1234567]

Raf I second the demo request,.

[aldepoalo]

Here is a link to the help files for script variables:

Mill Scripting Function Reference


Here is a link from the help files for the file extension to call up the different advance posting tabs:

Custom Variable Pages


Here is a quick video walk through showing how the advance posting tab works







And I have attached a sample post that uses the advance posting tab for your review.

http://bobcad.com/wp-content/media/p...ng-request.pdf

[RAF.]

Thanks Much Al

That was fast and some very good info
Thanks Again
RAF

[TonyW]

hey, I agree he should keep the files in bobcad edited to whats in the machine, but sometimes, that just isn't possible. lets take thread milling for instance. I have to manually add cutter comp to the file after bob posts the program, because it will not output a comp to threadmill, atleast not so far in my programs, ive done several threadmill jobs, and will be doing more. I am not going to run back and forth, trying to find out the right number that works, the easiest "workaround" I found is, just add the comp lines after I post it. but how am I supposed to update the program to something it doesn't even support? if you know, please share.

That's a post processor issue, Not a BobCAD issue. I had to edit a post for a special controller that uses different Gcode for cutter comp. Once that was set, all was good. It does comp just fine. Maybe I misunderstood what you typed, but getting comp to work isn't a big deal sometimes, just takes a little customizing to the post to get things the way you want it. I do thread milling all the time and it works fine. Just waiting for them to add tapered NPTF thread milling which they are working on. For that I just use Carmex's online gcode generator for their tools I use and paste the code into program using predator. Takes about 2 minutes.

[TonyW]

we are currently machining small aluminum wings with a 3d airfoil surface. we machine a single wing on a fixture in the middle of the table. production is increasing and we have the need to do 4 wings on a new fixture, but to fit within travels it is necessary to rotate the parts 90 degrees and translate to four positions. we have changed the program from a standard bobcad post to address some of the errors that were present. i need to copy the g code exactly as we are using it, just with different zero and xy coordinates.

thank you
keith

I think I misunderstood what you needed. If you already have the code do this, so long as your machine can do rotate, (on my Haas it's a G68 command for rotate), make 3 copies of your Gcode so you have 4 programs in one. in the first program section leave the G54 there. Search the second program and replace all G54's with G55 (Work coordinate 2). Search the third and replace with G56. The fourth, replace with G57. If your machine does not do rotate where you can just add the command at the start of each, you will have to rotate in Bobcad and get it how you want, generate the code for one working file, then do the above for each extra part. Then just zero out each fixture to each coordinate system. Would not be too hard to do manually. Hope that helps you