Other mastercam files, changing the control definition???

[Grimes]

Been forever since ive been on here...

 

trying to word this right

Ive seen this happen before, you load a file from a different mastercam program, and it seems to overwrite the control definition( im thinking). I was doing some of the tutorials off this site not blaming it, but after that the post changed. running an okuma 5 axis, and after that the machine wouldnt go to the home position. G30 P2. the post is encripted, so im sure thats not the problem. a few months ago i loaded a program from my previous shop. same kinda thing happened, just that time it changed the rapid movements to the part into a G1 at 5000 ipm if i recall. whats going on?

[JParis]

When you load a Machine def into a file, that file has it's own(local) version of the Machine & Control def....

You likely want to reload the machine into the file so that it picks up your latest version on that particular computer.

[crazy^millman]

Have to be careful with post defaults when it relates to misc reals and integers. Certain posts have them defaulted to defined values common for a certain machine. When you change the MMD and CMD the post will also be loaded in the Mastercam file. If they are different then the behavior they control when outputting like Home moves, tool changes and other things will be effected sometimes. This specific issue sounds like a misc real or integer in your post controlling how the machine goes home and because it is different you are getting different output. Where understanding theses switches and what they control are extremely important with 5 Axis post. Any 5 Axis post for Mastercam that does have them should have anyone running for the Hills. Yes I was in a shop a couple weeks ago and they had no control over what the post was outputting for code for their machines. 500 home moves in one program because they post builder thought they could take their knowledge of 3 Axis and use it for 5 Axis. 5 years the customer was doing this.

[JParis]

^^^^^^This^^^^^^

I go through this with the other programmers here...my HMC post iss very detailed with much functionality and flexibility bbuilt into the MI's & MR's...these guys get in trouble when importing ops they did on the VMC's and set them for the HMC, they forget to check those. Whereas I prefer to start all of my HMC programs with a fresh eye....I don't care how it was done on the VMC's, different machine, differant abilities and I want to leverage that in my programs....so many defaults come in pre-set.

To further illustrate Ron's point...

HMC

 

5 axis

 

VMC

 

As you see with the machines having different settings, when changing between amchines, you need to be aware of what "was" happening as compared with what "will" happen moving forward.

 

[Grimes]

6 hours ago, JParis said:

When you load a Machine def into a file, that file has it's own(local) version of the Machine & Control def....

You likely want to reload the machine into the file so that it picks up your latest version on that particular computer.

we tried that on friday same thing happened. right just been running one toolpath at a time.

3 hours ago, crazy^millman said:

Have to be careful with post defaults when it relates to misc reals and integers. Certain posts have them defaulted to defined values common for a certain machine. When you change the MMD and CMD the post will also be loaded in the Mastercam file. If they are different then the behavior they control when outputting like Home moves, tool changes and other things will be effected sometimes. This specific issue sounds like a misc real or integer in your post controlling how the machine goes home and because it is different you are getting different output. Where understanding theses switches and what they control are extremely important with 5 Axis post. Any 5 Axis post for Mastercam that does have them should have anyone running for the Hills. Yes I was in a shop a couple weeks ago and they had no control over what the post was outputting for code for their machines. 500 home moves in one program because they post builder thought they could take their knowledge of 3 Axis and use it for 5 Axis. 5 years the customer was doing this.

im assuming this is whats going on crazy, but how do i get it to post back the proper way. all the misc integers were at zero and my buddy teaching me the machine said to never turn them on because it can easily crash the machine.

2 hours ago, JParis said:

^^^^^^This^^^^^^

I go through this with the other programmers here...my HMC post iss very detailed with much functionality and flexibility bbuilt into the MI's & MR's...these guys get in trouble when importing ops they did on the VMC's and set them for the HMC, they forget to check those. Whereas I prefer to start all of my HMC programs with a fresh eye....I don't care how it was done on the VMC's, different machine, differant abilities and I want to leverage that in my programs....so many defaults come in pre-set.

To further illustrate Ron's point...

HMC

 

5 axis

 

VMC

 

As you see with the machines having different settings, when changing between amchines, you need to be aware of what "was" happening as compared with what "will" happen moving forward.

 

the work co-ordinates was set to a 2 when i opened up the control definition. but changing it back to a zero didnt change anything.

[JParis]

This might be one where contactin your reseller and letting them remote in may show them exactly what's happening...

[Aaron Eberhard]

20 hours ago, Grimes said:

we tried that on friday same thing happened. right just been running one toolpath at a time.

im assuming this is whats going on crazy, but how do i get it to post back the proper way. all the misc integers were at zero and my buddy teaching me the machine said to never turn them on because it can easily crash the machine.

the work co-ordinates was set to a 2 when i opened up the control definition. but changing it back to a zero didnt change anything.

I would start by reloading the post with Machine Group > files  > Replace.

Then, I would set your toolpaths to "Automatically set to Post defaults when posting" on the Misc Values page.

Finally, I would follow JP's instructions, and have a session with your reseller.  Your buddy is wrong, there's many many many times where those values will do anything from improve your surface finish to prevent a crash by orienting your machine the correct way when posting.  Learn how to use them.

 

[Grimes]

ya Aaron, we got it all sorted out. it was the "Automatically set to Post defaults when posting" problem first toolpath had it checked the other ones didnt. gonna try to look more into the misc values. but can they work with an encripted post, what ive seen is you might have to edit the post a bit to make them work?

[Aaron Eberhard]

4 hours ago, Grimes said:

ya Aaron, we got it all sorted out. it was the "Automatically set to Post defaults when posting" problem first toolpath had it checked the other ones didnt. gonna try to look more into the misc values. but can they work with an encripted post, what ive seen is you might have to edit the post a bit to make them work?

Glad to hear you got it sorted out :)

Yes, they can work with encrypted posts, but you won't be able to see the math behind what it's doing :)   That's where you'd need your post writer to include the options that you want.

To understand the misc values, think about the machine-specific situations you could be in. 

For example, you have a trunnion 5 axis table sitting on your vertical mill.  The tilt .  You need to machine something on the front of the part, so the trunnion needs to rotate the cradle (A axis) either +90 or -90.  If it tilts +90, the bottom of the cradle will be facing you.  If it tilts -90, the trunnion will be facing the back of the machine, and you can see the part.  Either solution is technically correct, and will machine fine, but you'd obviously prefer to see the part being cut @ A+90, right?  

That's where the Misc Integer "Initial Primary Angle" comes in.  If you type in 90 into there, when the post starts to figure out how to move the machine to get to the front face, it will start with the assumption that the A axis should be at +90. 

Another example would be if your machine has a smoothing setting, say it needs to output M250-M255. You can have a misc integer that lets you control which smoothing setting by typing in 0-5 into that field. 

Hope this helps!

[Grimes]

moving the tilt seems easier just to put -90 into the a-axis. thats what weve done in the past. so then the back face becomes the top face. if im understanding correctly what youre saying. Init. Rotary Axis Position is that the one youre talking about, maybe tomorrow i will test it on the machine thanks again Aaron.

[Grimes]

Just a question about the machine for anyone. an OKUMA mu-500 5-axis. they only run one home for everything. Co1 i guess, then when its tilting it switches to Co51. It has 100 homes in it, so it should be able to run that many different homes at once or not? we were running a fixture with four parts, they placed them in mastercam where they were on the fixture, im used to running each piece using a different home. just wondering if it is possible, or maybe not setup to do that. since nobody can see the machine i know its just guessing a bit.

[crazy^millman]

1 hour ago, Grimes said:

Just a question about the machine for anyone. an OKUMA mu-500 5-axis. they only run one home for everything. Co1 i guess, then when its tilting it switches to Co51. It has 100 homes in it, so it should be able to run that many different homes at once or not? we were running a fixture with four parts, they placed them in mastercam where they were on the fixture, im used to running each piece using a different home. just wondering if it is possible, or maybe not setup to do that. since nobody can see the machine i know its just guessing a bit.

Look for a switch in the post to not send it home. There should be switches to control this behavior when not needed. Okuma is a very powerful control and I don't think you need to send it home between indexes or multi axis moves.