Mastercam: transforming tool paths and multiple WPC's

[Freedommachine]

I've got some widgets I need to machine from a piece of plate. I created the geometry > created operations > transform tool paths in an array to get 30 pieces from each plate.

Now, I would like to add a second vise with a G55 work offset running the same operation, on the same material, for the same widget - sorted by tool # so that T1 will run G54 & G55 before the program calls up the next tool.

I imagine this is a fairly simple thing for proficient mcam users. I've still got training wheels on so I need a little assistance on this one lol. I'm running X9. Thanks!

 

[Barbter]

In your transform window, bottom left will be "Group NCI Output by Operation Order or Operation Type".
Have a clicky of this and it should work....
There used to be some youtube vids showing this. Be vigilant with transform though - it can be buggy if you transform a transformed toolpath etc.

 

[Mike1974]

what he ^ said. It's pretty straightforward when you know where to look. And if you click the help button in lower right a window should pop up showing the options and how they work.

 

[Freedommachine]

Yeah, I can't get it to work. I've read the all of the help info and it isn't very helpful in this case.

I don't know that a transform operation is what I need here. Transform wants to assign a specific distance, plane or other variable to manipulate the tool path.

I need to run the exact same tool paths, I just want to assign a second WPC for another vise without doubling my tool changes.

Is there a right way to do this in Mcam?
I'm not even sure what search terms might net results from the manual.

 

[Mike1974]

Have you cahnged the t-form type in lower left? Try clicking both options (not at once), then check your code. I am 100% you just have an option set wrong. It won't take long to see a difference in output.

That said, what version MCX? Are tour work offsets set so they output G54 etc, and not G92? I'ts an option somewhere, take screenshots and post?

 

[Barbter]

Try the attached.
Note: - my post is set to error on the standard 0,1,2 etc work offset designation for G54/G55/G5401/G5402 etc.
So if you see the lower right "box", it's set for Start 54, increment by 1.
You will prolly need start at 0, increment 1 (or start at 1, increment 1?).
The second page shows rectangular figure of 50,50 which is the pitch for a fixture plate (for example).
Bottom left of Instances (2 x 2) then outputs the qty 4 parts (G54/G55/G56/G57).
So have a play and shout.

 

[Mike1974]

Try the attached.
Note: - my post is set to error on the standard 0,1,2 etc work offset designation for G54/G55/G5401/G5402 etc.
So if you see the lower right "box", it's set for Start 54, increment by 1.
You will prolly need start at 0, increment 1 (or start at 1, increment 1?).
The second page shows rectangular figure of 50,50 which is the pitch for a fixture plate (for example).
Bottom left of Instances (2 x 2) then outputs the qty 4 parts (G54/G55/G56/G57).
So have a play and shout.

Good post! I forgot about setting saying something about the increment values.

Above that box (not to overload you sorry...) there is an option to ghost the original ops and copy them so everything is under one single transform op. There are other ways to do this for more advanced control, but this should cover the basics and what you are trying to do.

 

[Freedommachine]

Thanks for all the help guys.

Have you cahnged the t-form type in lower left? Try clicking both options (not at once), then check your code. I am 100% you just have an option set wrong. It won't take long to see a difference in output.

That said, what version MCX? Are tour work offsets set so they output G54 etc, and not G92? I'ts an option somewhere, take screenshots and post?

I think you're right about having the wrong settings selected. I played with it a bit using the screenshots Barbter shared for reference and I got it to generate the tool path. I still cannot get it to sort operations by tool # though. I'm thinking that might be a symptom of transforming an already transformed set of operations.

I am running MCX9. My work offsets post as G54 - G59.

My overall problem though is that I never started out learning Mcam the right way. I don't use tool groups, I don't make set up sheets, the tool library is whatever default came with the software...

I don't know how to do much other than draw a part and play with tool paths for hours until I reach a compromise that will result in the part I want.

From there, I post using a generic 3 axis fanuc file and then smooth out all the wrinkles manually in the .nc editor.

It works but it's very slow and inefficient compared to what mcam is capable of. I'm trying to be patient and struggle through the learning process that leads to proficiency but it's damn frustrating when time is money lol.

Try the attached.
Note: - my post is set to error on the standard 0,1,2 etc work offset designation for G54/G55/G5401/G5402 etc.
So if you see the lower right "box", it's set for Start 54, increment by 1.
You will prolly need start at 0, increment 1 (or start at 1, increment 1?).
The second page shows rectangular figure of 50,50 which is the pitch for a fixture plate (for example).
Bottom left of Instances (2 x 2) then outputs the qty 4 parts (G54/G55/G56/G57).
So have a play and shout.

Thank you for taking the time to put that together for me. Like I said; I was finally able to get it to generate the other set up, just not the proper tool order. I was a bit confused by the work offset designation box at first. Once I saw that you had it beginning at 54, I realized what was going on there.

I ended up just doing a copy / paste in the text editor for each tool operation and changing G54 to G55 for all of the copied text. It works but I'm going to keep messing with it in mcam to be sure I learn how to do it in the software instead.

 

[Barbter]

Bottom left "box" gives you toolpath making multiple parts then toolchange.
Or makes one part complete, then the next part complete.
I can prolly help you out with all you need for config files/machine and control def and post etc for X9.
Providing you gram in metric....

 

[Freedommachine]

Bottom left "box" gives you toolpath making multiple parts then toolchange.
Or makes one part complete, then the next part complete.
I can prolly help you out with all you need for config files/machine and control def and post etc for X9.
Providing you gram in metric....

That would be great, but brain only works in good ol' standard merican freedom units though. I don't do much metric

 

[dsj]

What I've done in cases like this is to transform each tool separately to do the parts on a plate, then transform all of the transformed toolpaths together to another WCS.

I'm sure there's a better way to word that, but it's Monday and early

 

[Mike1974]

That would be great, but brain only works in good ol' standard merican freedom units though. I don't do much metric

in your value boxes, type in (for example) 15.8mm. Working in the std english config start up, which I am pretty sure you are using, it will convert the 15.8mm to english units.

 

[Freedommachine]

What I've done in cases like this is to transform each tool separately to do the parts on a plate, then transform all of the transformed toolpaths together to another WCS.

I'm sure there's a better way to word that, but it's Monday and early

I gave this a try and it certainly got me closer.

I read over the help section a few more times attempting to understand exactly what all of the transform options do and I finally got somewhere this time.

I started by using Xform to create all of the widgets on the first piece of plate (G54). I then added those chains to each of my original tool operations.

For the G55 vise location; I transformed the original operations grouped by tool number - this worked well.

The next part I got hung up on was the second page of the transform op... where you enter the info to determine how and where the new tool path(s) will be placed.

I had to tell it a 'between points' distance and how many instances. Well, that doesn't help me here because I want to assign another work offset (G55) - not move the part with relation to WPC X0.Y0.

I just ended up offsetting my new transformed toolpath a total distance of 0.0. This created a new transform operation directly overtop of the original.

It worked, but you cannot see it in the Mcam workspace since they are on top of each other. Is this something you guys just deal with? Or do you place the transformed operations on a different level or something? (If that is even possible)

 

[Mike1974]

I gave this a try and it certainly got me closer.

I read over the help section a few more times attempting to understand exactly what all of the transform options do and I finally got somewhere this time.

I started by using Xform to create all of the widgets on the first piece of plate (G54). I then added those chains to each of my original tool operations.

For the G55 vise location; I transformed the original operations grouped by tool number - this worked well.

The next part I got hung up on was the second page of the transform op... where you enter the info to determine how and where the new tool path(s) will be placed.

I had to tell it a 'between points' distance and how many instances. Well, that doesn't help me here because I want to assign another work offset (G55) - not move the part with relation to WPC X0.Y0.

I just ended up offsetting my new transformed toolpath a total distance of 0.0. This created a new transform operation directly overtop of the original.

It worked, but you cannot see it in the Mcam workspace since they are on top of each other. Is this something you guys just deal with? Or do you place the transformed operations on a different level or something? (If that is even possible)

to make a second/third wcs, just make the transform at 0,0 and on the first page select assign new for wcs. unless there is something else going on, this is the way I have always used for a generic Haas post