Yes. Just create a cs for each vise and create your processes in the appropriate cs.
I'm finding the documentation on Work Fixture Offsets a little sketchy. Say I wanted to emulate a 4 vise set up as in the pic below. Can I tell GibbsCAM that each of those rectangles represents a seperate work offset, even though they are in the same plane?
Yes. Just create a cs for each vise and create your processes in the appropriate cs.
OK. Here's my attempt to do that and to try and understand a few things about CS's. My example is simple, and artificial. I've created 2 new CS's (I called them G54 and G55), both of which initially copy CS1 (XY plane). I've drawn a rectangle in each CS, moved the origin (X0Y0) of each CS to the middle of the rectangle, and drilled a hole at X0Y0. Here's my CS's:
When I click on CS 1, the default CS, I see this:
When I click on G54, I see this:
When I click on G54, mod (1), I see this:
When I click on G55, I see this:
And when I click on G55, mod (1), I see this:
I have 2 main questions:
1. Why are "G54, mod (1)" and "G55, mod (1)" created when I move the origin, leaving the geometry stored in the original version, and the origin markers displayed in the modified version?
2. Do the points I have placed at the "origin" of G54 and G55 really represent absolute X0.Y0. for the respective CSs? If so, why does the generated code not drill at X0.Y0. It drills at X-2.5 Y0. and X2.5 Y0., respectively, which are absolute coordinates relative to CS 1's origin, not G54 and G55's origin. Whats up with that?
Any clarification of these two issues would be greatly appreciated.Code:% ( TOOL 1: .5 DRILL ) S1000M3 G90G0X-2.5Y0. G43Z1.H1T1 M8 Z.1 G83G99X-2.5Y0.Z-2.R.1Q.05F4. G0G80Z.1 ( TOOL 1: .5 DRILL ) G90G0X2.5Y0. G83G99X2.5Y0.Z-2.R.1Q.05F4. G0G80Z.1 M9 G91G28Z0. G90 M5 G28Y0 M30 %
I should mention that I have discovered the Post Processor dialog box's Number of Parts text box and One Part All Tools radio button. I can, for example, draw 2 "parts" in the default XY plane, and tell my post processor to generate code for 2 parts. When I do, I get G54 and G55 work offsets in my code. But thats using 1 coordinate system, the default.
I'm just trying to gain a better understanding of how multiple coordinate systems work, and how using them could be advantageous in (primarily) 3 Axis Milling (though we also have 2 horizontal mills with B axes).
Question 1 - You have one or more options checked in the CS Preferences. By default, when you move an origin anything created while it is active moves with it. Right click on the CS List to bring up the Preferences menu. Here you will find options for handling geometry & toolpaths when you move an origin.
Question 2 - You created both drill processes in CS1. Open each process box and in the bottom right corner you'll see Mach. CS: and a dropdown list that will display all of the CS in the file. You need to select the one you want to machine in to output correctly.
The Number of Parts option is really meant for outputing multiple work offsets for parts that are fixtured the same, like four parts in four vises located the same way, etc... .
OK, here's take 2.
I did the following in the following order:
- Created 2 user CSs (G54,G55) both based on (copies of) the default XY Plane.
- Moved the origin of G54 and G55 to the left and right, respectively, of the default origin.
- Created some geometry (a single point) in each user CS. The point is located at X0.Y0. of each user CS.
- Created a process to drill the point in each user CS. The appropriate CS was selected for each process.
The default axis marker is showing, frame indicators for G54 and G55 appear, and tool path is displayed for P1 (identical tool path for P2).
I feel like thats all set up correctly.
I can't get my post processor to recognize and emit code for my two user coordinate systems. I was kinda' hoping to see a G54 work offset and a G55 work offset in my code, with drilling going on at X0.Y0. in both work offsets. Instead everything is still oriented relative to the default XY plane.
Is what I am looking for something that is controlled by the post, and I just don't have a post that can do that? Or am I not doing something correctly in GibbsCAM?Code:% O1100( PROGRAM: WORK_OFFSETS_3.NCF ) ( FORMAT: MXXX_12 VERTICAL.PST ) ( 8/10/11 AT 6:45 PM ) ( OUTPUT IN ABSOLUTE INCHES ) ( PARTS PROGRAMMED: 1 ) ( FIRST TOOL NOT IN SPINDLE ) N1G17G80G40 G54X0Y0Z0 T1 M6 ( OPERATION 1: HOLES ) ( WORKGROUP ) ( TOOL 1: .5 DRILL ) S1000M3 G90G0X-4.Y0. G43Z1.H1T1 M8 Z.1 G81G99X-4.Y0.Z-2.5R.1F4. G0G80Z.1 ( OPERATION 2: HOLES ) ( WORKGROUP ) ( TOOL 1: .5 DRILL ) G90G0X4.Y0. G81G99X4.Y0.Z-2.5R.1F4. G0G80Z.1 M9 G91G28Z0. G90 M5 G28Y0 M30 %
Thanks, as always.
You need an Advance Mill post when using coordinate systems. The format code in your sample is not an Advance Mill post label. To post using PostHaste you would also need to upgrade the PostHaste plugin.
Other than the post issue, your example looks fine.
If I had an Advance Mill post, would my code output show 2 drilling operations, one at G54 and one at G55, both drilling at X0.Y0.? I'm just curious what it would look like. Or would it look like whatever we designed it to look like? I know very little about "posts" and how they come to be. I do have a lot of posts that I was given, however. Is there anything specific in the format that would indicate to me I was looking at an Advance Mill post? I could look through the posts that I have for one.
Without an Advance Mill post, is there really much point in using coordinate systems in 3 axis vertical milling? It seems to me that using coordinate systems might come in handy, however, programming on horizontal mills where B axis rotation is involved.
What is PostHaste?
Last edited by eliot15; 08-11-2011 at 06:03 PM.
With an Advance Mill post your code output will be correct. The code will be relative to the CS you machine in. This is especially important when indexing around a rotary axis.
Heres a link that explains the label definitions:
Welcome to the GibbsCAM Support Center
You can do simple 4 axis positioning in the basic mill package, so you don't need an Advance Mill post to do that. If you need a post modified, the post department at GibbsCAM will help you out.
PostHaste is the built in third party plugin that allows you to create and modify post templates yourself. It is not the same as the internal post engine & .pst files. What version of Gibbs are you using? If you have a really old version, like V5.xx, you won't have it.
I'm running version 9.5.1 32 bit. We have 2011, but I don't have it installed yet.
I see that I do have PostHASTE installed with a pretty extensive template library. I just kicked out a random NC file. I'll have to play with that a bit.
Thanks a million for all the help on this issue. I'm hoping working with multiple coordinates systems will help us program our horizontal mills down the road. We also just picked up a PUMA Turn/Mill which should be interesting to work with.
I printed out the info. at the Gibbs Support link. I'll take it to work today and see what we have post-wise.
I bought the PostHaste 5 axis upgrade about 5 years ago but don't use it now. I had my post modified for our 5 axis machine and it works really well.
When I bought my seat it came with B, C, & D Advance Mill posts, so you should have one. Get your copy of 2011 installed.
Well shut the front door!! After a bit of digging, turns out we have a small boat load (about a dozen) Fanuc Advanced Mill posts (mostly B with a C or two).
Here's what I've been after. Same program we've been kicking around:
Yee ha. Thats me drilling at X0.Y0. in two different user defined coordinate systems.Code:% O1100( WORK_OFFSETS_3.NCF ) ( FORMAT: FANUC 11M B007.16.PST ) ( 8/12/11 AT 5:53 PM ) ( OUTPUT IN ABSOLUTE INCHES ) ( PARTS PROGRAMMED: 1 ) ( FIRST TOOL NOT IN SPINDLE ) N1G17G70G80G40 T1 M6 ( OPERATION 1: HOLES ) ( WORKGROUP ) ( TOOL 1: .5 DRILL ) ( CS#1 - G54 ) ( G54 = X-4. Y0. Z0. ) G54 S1000M3 G90G0X0.Y0. G43Z1.H1 M8 Z.1 G81G99X0.Y0.Z-2.5R.1F4. G0G80Z.1 ( OPERATION 2: HOLES ) ( WORKGROUP ) ( TOOL 1: .5 DRILL ) ( CS#2 - G55 ) ( G55 = X4. Y0. Z0. ) G55 G90G0X0.Y0. G81G99X0.Y0.Z-2.5R.1F4. G0G80Z.1 M9 G91G28Z0. M30 % ( FILE LENGTH: 561 CHARACTERS ) ( FILE LENGTH: 4.95 FEET ) ( FILE LENGTH: 1.58 METERS )
Kinda' interesting, though, that the code format contains a comment that defines each CS's origin in terms of its position relative to the default XY origin. G54 is X-4. Y0. Z0. and G55 is X4. Y0. Z0.
I'll have to see what my other posts kick out.