MasterCam X Multiple Fixtures

[MachiningPartne]

Thank you all in advance.

I am trying to make identical parts on multiple fixtures. Using Fadal its E1,E2,E3,E4 (G54,G55,G56...) on 4 vises. So 1 part per vise using different XY 0. I want Each tool to complete all its operations before moving to next fixture.

I have tried few options but seem to be missing something.
I have managed to make multiple fixtures using "Transform Toolpath" but the issue is it runs Each Operation than moves to another fixture, than moves back to first and runs another operation and so forth. I want the entire tool to finish running on 1st fixture before moving to fixture two.

For Example If I have T1 Shell mill contour at Z0 and contour at Z-.2. The Toolpath transform will cut Z0 on E1, than move to E2, than E3... after that it will go back to E1 and run Z-.2, than move to E2, E3 and so forth. Now imagine that with 15 different pockets depths.

That cuts down on productivity due to additional moves between fixtures.

I also tried View Manager but frankly I get confused in it and it appears to have similar issue where I would have to copy each cut and assign work offset to it.

Additionally I tried sending out subroutine but it also creates subroutine for each operation rather than tool.

I can make subroutines by hand but working with fairly large NC files its very time consuming and easy to mess up.

If you guys have any suggestions please let me know, maybe even screenshots :-)

thank you,

[txcncman]

You were in the right place. You just need a little help flipping the right switches.

Go to Toolpath - Transform. Type - Transform - Tool Plane Origin Only. Method - Tool Plane. Select the source operations (Ctrl+Click). Unselect - Create New. Select - Copy Source, Select - Disable posting, Unselect - Subprogram. Work Offset Numbering - Assign New - Start - 0 - Increment - 1. Group NCI - Select - Operation Type.

Translate Tab. Translate - Rectangular. X spacing - 0, Y spacing - 0, X steps - 4, Y steps - 1.

If that does not work for you, let me know. I have another trick up my sleeve.

[Geof]

Wade your way through this thread:

http://www.cnczone.com/forums/master..._fixtures.html

Partway through DonkeyHotey has it all worked out.

[Delw]

I found it easier:
if you are cutting jaws and your vices are in line and true and also have a Known set distance then program one vice and copy the parts 3 times so you have all the same E number.

if you dont have enough memory
then use sub programs with different fixture offsets.
Subs are very easy on a fadal to use.
the only time you may have a problem with subs is if you have tight tols and your table is slightly out of wack on one side you cant adjust each individual part for compensation.

I have a ton of memory in the fadals so I just program it and copy everything, and I use a deadicated rougher and finisher for all machining. granted the programs are long.

Delw

[MachiningPartne]

Thanks , but it seems to do same thing. I tried before same as you suggested except selecting Tool plane origin only and I used same amount of X/Y steps in the translate tab.

By the way not sure if it you meant - (minus) in the x/y steps because I can put only positive numbers and in the Type field I have
- Translate / tool plane only
- Rotate
- Mirror
I do not have "transform" in the Type field.

It still does not complete all operations for each tool but finishes 1st operation T1, moves to next fixture...than comes back again to 1st fixture finishes second operation, move to next fixture and so on. Maybe there is an option to group operations into main "tool operation" or something along those lines.

Man, there sure are so many options Mastercam. :-) I almost miss Geopath and GeoPromt and its simplicity -
Enter number of Fixtures: 4
done, :-)

I will also go thru the other suggestion given here, thank you guys for pitching in. But I really think there has to be an easy way within the software without messing with NC file or having to use exact distance vises etc. Given the price-tag you would expect something as common as this to be part of options without having to hand edit and look for work arounds.

You were in the right place. You just need a little help flipping the right switches.

Go to Toolpath - Transform. Type - Transform - Tool Plane Origin Only. Method - Tool Plane. Select the source operations (Ctrl+Click). Unselect - Create New. Select - Copy Source, Select - Disable posting, Unselect - Subprogram. Work Offset Numbering - Assign New - Start - 0 - Increment - 1. Group NCI - Select - Operation Type.

Translate Tab. Translate - Rectangular. X spacing - 0, Y spacing - 0, X steps - 4, Y steps - 1.

If that does not work for you, let me know. I have another trick up my sleeve.

[txcncman]

The dash was a separator, not a minus sign.

I think I understand your issue a little better now. Not sure why you just did not post your MCX file to begin with. Would have made sorting through the forest to find the trees much easier.

Use WCS Manager and copy your tool plane 4 times. Rename the new tool planes E1, E2, etc. Give Work offset numbers 1, 2, etc. for each tool plane.

In Operations Manager, highlight all ops. Right click and the click Edit selected operations - Edit common parameters. Click Planes checkbox. Select E1. Uncheck Display relative to WCS. Propogate E1 to the right for all planes. Click ok. Click ok. Regen ops.

Make copy of ops and paste in Operations Manager. Highlight these new ops and change to E2.

Repeat for E3, E4, etc.

Highlight all ops, including new ones. Right click. Click Sort - Sort. Sort by Tool number. Click ok.

Highlight all ops. Right click. Click Edit selected operations - Change NC file name. Change as needed. Click ok.

Highlight all ops. Right click. Click Edit selected operations - Change Program #. Change as needed. Click ok.

This should put all your tool 1 ops together and in order of E1, E2, etc. At this point you can move them around to adjust if needed.

[WallyL7]

I believe what you need to do is just transform each tool...

so,

At the end of the program you can add a single transform toolpath for each tool - including all of it's toolpaths.

So, if your toolpath(tp) manager looks like this

(tp)
#1 drill - tool1
#2 drill - tool 1
#3 drill - tool 1
#4 contour - tool 2
#5 contour - tool 2
#6 contour - tool 3


add in
#7 transform (select tp #1,2,3) (just tool 1)
#8 transform (select tp #4,5) ( just tool 2)
#9 transform (select tp #6) ( just tool 3)

I think you have your transform parameters set up correctly already (based on what guys have already said here), so that should work for what you want if I understand you.

In other words you are grouping each tool in its own transform and in the order you are running your program - so if you go back to a tool later in the program, it will need another transform in that location.

[txcncman]

After going back and re-reading your first post, why the heck are you cutting to Z0. and then Z-0.2 with a shell mill in 2 different ops? One assumes you are facing your material. Why the heck didn't you use Depth Cuts option to complete in 1 op? Same thing for pocketing?

[MachiningPartne]

No no, I used Z0 / Z-.2 just as example to explain I used same tool for different operations, like I have 1/2EM cut outside contour, than few bigger pockets with depth cuts etc. Also there are 24 pockets with different depths, that is why I needed this. The shell mill just faced top.

Anyways,
I tried using View Manager to create multiple fixtures and it worked great. The key was to sort them by tool after all ops were copied and assigned fixture #.

Thank you Very Much.

After going back and re-reading your first post, why the heck are you cutting to Z0. and then Z-0.2 with a shell mill in 2 different ops? One assumes you are facing your material. Why the heck didn't you use Depth Cuts option to complete in 1 op? Same thing for pocketing?

[kprice1658]

I do this all the time, just by using transform toolpaths, translate between points - setting that number to the number off offsets, like 4 for G54-G57.

I think the key to your problem is the "group NCI output by" - controls the tool operation order. Set that to control the operation order between the different vises (origins).

As usual, there are several ways to get there, each has their own flavor...

[txcncman]

@kprice - I could be wrong here, but I think using your method would give one of two results. First would run process #1 on each vise in order G54, G55, G56, etc. Second option would run all processes on vise #1, then run all processes on vise #2, etc. If process #1 uses tool #1 and process #2 also uses tool #1. Either of these scenarios creates some wasted movement. In the first scenario, tool #1 would jump from vise to vise for process #1 and then have to jump back to vise #1 for process #2. In the second scenario, all tools would run on vise #1 and then have to go back and reload tool #1 and jump to vise #2 to run all of the tools again. Lots of tool changing on this scenario.

Yes, programmer/machinists can do things anyway they want as long as they can produce results good enough to get paid for. But, there are "best practices". Ways of doing things that are more successful and more efficient than other ways.

[kprice1658]

txcncman,

I do it that way everytime I have multiple offsets. I never have to copy operations. All operations that use the same tool run in each offset, then, tool change, next OPs run.

Say my OP1, OP2 and OP3 both use tool1, and OP4 & OP5 use tool2, and there are 4 offsets, G54-G57. I use a custom made jig to hold up to 6 offsets and set them with a probe.

OP1,2,&3 (same tool)will run at G54, move to G55, then to G56 and so on til done.

Tool change to tool2, then OP4 &5 (same tool) both run on G54, move to G55, etc..

Less tools changes and less travel. At least this way works best for me.