Tool Path Transform Work offet numbering?

[neurosis]

Ive always wondered about this but have never asked.

 

When transforming a tool path using Tool Plane Method, When you set the Work offset numbering to OFF, is is supposed to suppress work offset numbering? Because it seems to still add a fixture offset number for every rotation ( I am using transform rotate in this example ).

 

The help says,

 

Off

 

Does not output any work offset codes for the transformed operations.

 

 

Am I misunderstanding what it is telling me?

[Dave.L]

Ive always wondered about this but have never asked.

 

When transforming a tool path using Tool Plane Method, When you set the Work offset numbering to OFF, is is supposed to suppress work offset numbering? Because it seems to still add a fixture offset number for every rotation ( I am using transform rotate in this example ).

 

The help says,

 

 

 

Am I misunderstanding what it is telling me?

 

 

The source OP will still output a workoffset but the transformed OP should not.

[neurosis]

Well the Source OP is outputting a fixture offset ( you must have a fixture offset to begin with ) but all rotations are outputting different fixture offsets. This has been happening to me since I started using Transform operations.

 

In previous versions I was able to fool the system in to not outputting offsets by changing Work offset numbering to Assign new and then leaving the values at 0, 0 but this does not work in X5. Im having a hard time figuring out how to fool X5 in to doing what I want.

[Dave.L]

Well the Source OP is outputting a fixture offset ( you must have a fixture offset to begin with ) but all rotations are outputting different fixture offsets. This has been happening to me since I started using Transform operations.

 

In previous versions I was able to fool the system in to not outputting offsets by changing Work offset numbering to Assign new and then leaving the values at 0, 0 but this does not work in X5. Im having a hard time figuring out how to fool X5 in to doing what I want.

 

 

It might be something in your post. I use the transform function only to do multiple parts on a fixture and I always want different fixture offsets, so I can help much with your issue - it might be a bug.

[neurosis]

It happens with every post that I try. Ive tried about 10 different Machine Defs and Posts just to make sure.

[neurosis]

I may need someone to explain these for me. I realize that my reading comprehension could be better but what should I take away from these explanations?

 

 

Off

 

Does not output any work offset codes for the transformed operations.

 

 

This one has me a little confused because I am not sure how it would differ from "Maintain Source Operation". Regardless of my understanding of this explanation, it DOES output a different work offset for EVERY rotation.

 

Maintain source operation

 

Uses the work offset settings from the source operation for each transformation. Only available for translate and rotate toolpaths using the tool plane method.

 

 

I would assume that every rotation should use the same fixture offset? I.E. if the source operations are using G54 it would = G54 for every rotation? Again, I get a different Work Coordinate for every rotation.

 

Match existing offsets

 

Checks to see if any of the work offset views that are created when the toolpath is posted match any existing or predefined views.

 

If the views match, then the existing view is used.

 

If the views do not match, the new work offset view is created.

 

 

 

That one I think that I just might understand. Although it seems to do this no matter which selection I make.

 

 

 

 

And I was wrong. I get the same results whether I use a previous version of Mastercam or X5 when using rotate.

[André Lapointe@In-House Soluti]

I think the help file is not clear enough in this case.

Based on my experience when you set it to OFF and that you don't have a change in your toolpane orientation no work offset should output, but if you do a rotate for example, you are going to use a different toolpane for every instance. And if you are using the option OFF, it tells mastercam to use the default option, which is to increment the work offset number for every different toolplane.

The easiest way to get what you want , is to set it to Assign New, set your starting work offset (the same as your source operation) and put the increment value to 0.

This way you will never get incremented. That's the way I usually do it.

HTH

 

 

[neurosis]

When you are doing as you explain, are you also having to change the default Work Offset numbering in your View Manager from -1 to which ever work offset you plan on using?

 

I ask because that is the only way that I have ever been able to get that method to work. Otherwise it still continues to output a different wcs for every rotation.

 

And I agree. The help file is either not clear enough or this is not working properly assuming that I am understanding what it is saying. Your explanation of "OFF" makes sense to me but I am still confused by "maintain source operation".

[André Lapointe@In-House Soluti]

I don't remember having to set the work offset prior the transform.

I just tried it again, with a rotate transform around the X axis 3 copy and I usually choose to copy the source operation within my transform.

Set the work offset numbering to Assign new, start 0 increment 0 and I get only G54's all the way down.

[neurosis]

I am currently playing with a part in X4MU3 and I cant get it to work UNLESS I change the work offset to 0. I am getting some strange results today.

 

Settings

 

Work Offset -1

Rotate

Transform Method Tool plane

Work offset numbering Assign new, Start 0, Increment 0, Match existing offset ticked.

 

It changes my original wcs to g55 and then the transformed operations to g54.

 

N1 T1 M06 ( 2 INCH INGERSOL FACEMILL)
G00 G17 G90 G55 A0. X-4.1865 Y-1.6084 S764 M03
G43 H1 Z3. T2
Z.8625
G94 G01 Z.7725 F50.
Y1.6084 F15.28
G00 Z3.
G91 G28 Z0.
M01
G00 G40 G49 G80 G90
N2 T2 M06 ( 3/8 SPOTDRILL)
G00 G90 G55 A0. X-4.28 Y0. S458 M03
G43 H2 Z3. M08 T3
G98 G81 Z.6875 R.8625 F1.83
G80 M09
G91 G28 Z0.
M01
G00 G40 G49 G80 G90
N3 T3 M06 ( 3/8 DRILL)
G00 G90 G55 A0. X-4.28 Y0. S458 M03
G43 H3 Z3. M08 T1
G98 G83 Z.2998 R.8625 Q.1125 F2.29
G80 M09
G91 G28 Z0.
M01
G00 G40 G49 G80 G90
N1 T1 M06 ( 2 INCH INGERSOL FACEMILL)
G00 G90 G54 A180. X-4.1865 Y-1.6084 S764 M03
G43 H1 Z3. T2
Z.8625
G01 Z.7725 F50.
Y1.6084 F15.28
G00 Z3.
G91 G28 Z0.
M01
G00 G40 G49 G80 G90
N2 T2 M06 ( 3/8 SPOTDRILL)
G00 G90 G54 A180. X-4.28 Y0. S458 M03
G43 H2 Z3. M08 T3
G98 G81 Z.6875 R.8625 F1.83
G80 M09
G91 G28 Z0.
M01
G00 G40 G49 G80 G90
N3 T3 M06 ( 3/8 DRILL)
G00 G90 G54 A180. X-4.28 Y0. S458 M03
G43 H3 Z3. M08 T1
G98 G83 Z.2998 R.8625 Q.1125 F2.29
G80 M09

 

Keep in mind that this is just me testing some things out to try and understand how this works a little better so the program and indexes are a bit unorthodox.

 

I am just transforming three tools to do the same thing on the 180 face of a part and this is my results using the above parameters.

 

I am not using copy source operations. I am just keeping the original and then using a transformed path for the 180 side.

 

If I change the Work Offset to 0 it will output all G54.

[André Lapointe@In-House Soluti]

If you don't copy the source operation this may make some sens because you are leaving the work offset to -1 which is not recommended because it lets Mastercam decide and increment the generated value based on the use of the toolplane.

If you copy the operation in it, you won't get this problem.

 

Now I don't know how you could do it without having to set it in the source operation without having Mastercam to increment it.

 

 

 

 

[neurosis]

It would be nice if there were a very clear setting that would output a single WCS only. It seems like there are too many hoops to jump through to get something so simple to happen.

 

Tip your hat sideways, hold your leg up, spin your coffee cup handle to the left, part your hair down the center, and THEN you will get the correct WCS output.

 

And just so we are clear in all of this, I am using MPMaster and I do know that there is the Misc Inter "Lock on first WCS". I am just trying to understand the thinking behind how the Transform WCS numbering goes. It seems that you should not need a Misc setting to accomplish this? I notice that some of the default posts do not have this option in them.

[Russh67]

Hi:

 

This is my first attempt to help some one so I hope I'm correct.....

 

I do this also frequently. What I do is the following:

 

-Go to the Misc values page and un-check the box where it says "Automatically set to post values when posting" box.

 

-in your operations go to the planes page and set the work offset numbering to 0. leave the relative to WCS box checked.

 

-then in the transform page under method check tool plane, include origin and save views. Also ckick copy source operations and disable posting. Under work offset numbering click asign new and leave start and incriment to 0. I also have the operation type clicked and NCI as the source.

 

-Under the Rotate tab I clicked rotation view and used my own defined WCS. Also 1 instance and both angles at 180, which you probably did already.

 

I have found in general that in regards to controlling work offsets un-checking the automatically set to post values when posting makes a big difference, especially in lathe. I am not sure but I think it the work offset settings in the post..

 

Let me know if I helped you or if I drove you more crazy....

 

[Russh67]

Hi:

 

This is my first attempt to help some one so I hope I'm correct.....

 

I do this also frequently. What I do is the following:

 

-Go to the Misc values page and un-check the box where it says "Automatically set to post values when posting" box.

 

-in your operations go to the planes page and set the work offset numbering to 0. leave the relative to WCS box checked.

 

-then in the transform page under method check tool plane, include origin and save views. Also ckick copy source operations and disable posting. Under work offset numbering click asign new and leave start and incriment to 0. I also have the operation type clicked and NCI as the source.

 

-Under the Rotate tab I clicked rotation view and used my own defined WCS. Also 1 instance and both angles at 180, which you probably did already.

 

I have found in general that in regards to controlling work offsets un-checking the automatically set to post values when posting makes a big difference, especially in lathe. I am not sure but I think it the work offset settings in the post..

 

Let me know if I helped you or if I drove you more crazy....

[MrFish]

We had our post adjusted to ask a question for what work offset number to use - it then outputs this number at every offset call.

 

This is a great insurance feature to make sure that you are using the same offset through out your program, especially important when posting 4 and 5 axis work and you forget to set your tool/construction plane when using custom WCS.

 

Also gets around this issue of mastercam indexing the offset number when using transform or rotate toolpathes.

 

By the way we also have a copy of the post without this feature for when we require multiple offset positions for multiple setups.

[neurosis]

I appreciate the effort Russh.

 

 

My goal here is to get a better understanding of the intended use of Work Offset Numbering in Transform.

 

I have a few parts that are very simple indexer jobs. I program them using Transorm Rotate but the caveat is, I do not have a post that outputs correct code for our HAAS Indexer (uses M20) and I am too lazy to modify one. For a couple of different reasons.

 

What I end up doing, is creating path and then using a Manual entry to place the M20 and a comment in to the program at the index. I know that this would not be a preferred method but for the few jobs that we do on that particular indexer it works and it is simple. This method also does not allow me to use "Copy Source Operations" so I am stuck with having to figure out how to get the correct output without it.

 

I figure that if I can get a better understanding how to use that area of Transform properly I wont have to jump through so many hoops due to the various different machines and posts that we have and use.

[Russh67]

Neurosis:

 

Where does the m20 go??

 

I have noticed in x5 that "automatically set to post values" thing changes how offset are numbered..I think that with that checked it will post according to the post values for offset numbering. If I uncheck it then the transform behaves a little more like I expected. Still does not match the help files that you quoted though.

 

I have had to repost jobs for minor feed or peck drill changes and noticed I was getting g55 and g56 appearing were they weren't before...with x5....x5 is buggy.

[neurosis]

I add the M20 using a Manual Entry between the operations that I created and the Transform operation/Rotation. This only work for some things and is very limited!

 

 

Automatically set to post values, and someone please correct me if I am wrong, resets your Misc Values to what ever they are set to in your post. By deselecting this, you can change your Misc values to use what ever functionality you have added to them in your post. It is a very nice feature of Mastercam. When I first started to use Mastercam I had no idea what a Misc Integer or Real was. Now my thinking is that there are not enough of them.

 

Im not sure what post you are using, but if it has an option similar to Mpmasters "Lock on First WCS" then it would explain the difference in your output by merely deselecting that check box.

 

Im not sure whether the Work offset numbering in transform works as intended or not. The help files are too vague and I have never had each of the functions intended use explained to me so it leaves me to interpretation. Which I have found never works in my favor when trying to figure things out inside of Mastercam.

[Russh67]

Neurosis;

 

Interesting... I do not have "Lock on First WCS". I tis a post ive been using since 07 when we bought the machine. It a copy of the generic Haas post with x3 or x2 I think with some changes I made with the help of our reseller..

 

Any way this is fun...thanks for breaking me in....

[Dave.L]

Neurosis,

 

I know your issues are different, but maybe this will help you, maybe not:

 

http://www.emastercam.com/board/index.php?showtopic=37447&st=0&p=274178&hl=+tech%20+tip&fromsearch=1entry274178