motor-vater

5 axis Tool paths and Planes?

Recommended Posts

When doing a 5 axis curve/ Swarf or any multiaxis path for that matter is it always Top/Top/Top? I ask cause I have been fumbling around 5 axis for about 10 years and always used T/T/T but some times get real undesirable entry motions and exit motions, but recently did a curve from a plane I didn't realize I was on and it still worked fine. So what are you guys doing? Have I been going at this all wrong for years? lol

 

Share this post


Link to post
Share on other sites

We always use our "5 axis home" which is basically top top top.

 

It may work otherwise, but our dealer recommend to use the a0c0 wcs

Share this post


Link to post
Share on other sites

Top/Top/Top (or, the home plane) is all I've ever used. I was told, by the guy that tutored me, 5X paths can only be programed from here.

Share this post


Link to post
Share on other sites

The planes are being respected by the traditional backplot, but that may not be the same as what you see on the machine. I am not sure if the new backplot engine that does the verify cares about the planes as I never use it. I work with a lot of different machines and do a lot of different work so planes and WCS are my friend. I have found the biggest thing with the 5 axis toolpaths is just know what you know and control what your not sure about and everything from that point is not a problem. T/T/T it not required for many versions and yes years ago that was the only way, but major improvements have been made to make Mastercam WCS aware why we lost the ability to change the name and positions of the base planes. When they locked that down they gained the control needed in the software to have a base point for reference that was lacking. We start talking about DWO and TCP and use the machine to control the COR as it should be and now we really see T/T/T is not important either. Yes still many that have this ability with their machine programming COR and have to repost anytime the part moves from the COR verses using the machine the way the technology was meant to be used to help them be more efficient. Seems off topic, but it is all related. With the Moduleworks toolpaths pay close attention to your linking and you will see how much that control your in and out motion and how certain settings can hurt or help your process. 

Share this post


Link to post
Share on other sites

Yep, as Ron said, starting with X9, all of the multiaxis toolpaths became WCS aware...  That was my first release as the Product Owner *sniff* :)  Back when I trained you (X4?), it was REALLLY important to always have a multiaxis toolpath set in the Top WCS.

Basically, a plane is more or less irrelevant to a multiaxis toolpath (if you have one curve toolpath that starts on the front and then continues around on the side, what "plane" is that toolpath on?"), but the WCS is really important to us.   Changing from T/T/T to T/F/F will only change the way the data is stored in the background NCI (if you care, it goes from saving it as XYZIJK to XZYIKJ).  Because of the way you were digitizing on the machine at the time, the that plane inversion would alter the commanded positions of the probe, so on a digitizing Flow 5 Axis toolpath, it was REALLLY important make sure it was in Top/Top/Top before posting.

So the important thing to remember nowadays is that whenever you interact with an X,Y,Z in a multiaxis toolpath (Lock to 4 axis and rotate around Y, Limit the XZ plane motion, Fixed Angle to X, Retract Along Z, etc.), all of those X Y Zs are relative to whatever WCS the toolpath is in. 

 

Share this post


Link to post
Share on other sites

Awe!!! Arron you remember the version and everything! Man have we come a long way my friend.... It seems like those early lessons have carried me very far, and I am grateful, and glad you are still here for me. But yes the game has changed, I was just blown away the other day when I posted something out and ran it trough vericut and then the machine with no problems, then when I went back to modify a few things I realized my planes were not at T/T/T, or my New top/ New top, New top in that case and I was like Wow! OK

  • Like 1

Share this post


Link to post
Share on other sites

What about machines where the "0,0" view is not top?? Top view on one of our 5 axis machines would be b90. - c90. 

Share this post


Link to post
Share on other sites
1 hour ago, navsENG said:

What about machines where the "0,0" view is not top?? Top view on one of our 5 axis machines would be b90. - c90. 

Not a big deal your post will do all the heavy lifting. Really comes down to how you need to define top? Does it need to be T/T/T or F/T/T? I have worked with many different configurations over the years and the post is what drives this not Mastercam anymore. 

Share this post


Link to post
Share on other sites
23 hours ago, 5th Axis CGI said:

The planes are being respected by the traditional backplot, but that may not be the same as what you see on the machine. I am not sure if the new backplot engine that does the verify cares about the planes as I never use it. I work with a lot of different machines and do a lot of different work so planes and WCS are my friend. I have found the biggest thing with the 5 axis toolpaths is just know what you know and control what your not sure about and everything from that point is not a problem. T/T/T it not required for many versions and yes years ago that was the only way, but major improvements have been made to make Mastercam WCS aware why we lost the ability to change the name and positions of the base planes. When they locked that down they gained the control needed in the software to have a base point for reference that was lacking. We start talking about DWO and TCP and use the machine to control the COR as it should be and now we really see T/T/T is not important either. Yes still many that have this ability with their machine programming COR and have to repost anytime the part moves from the COR verses using the machine the way the technology was meant to be used to help them be more efficient. Seems off topic, but it is all related. With the Moduleworks toolpaths pay close attention to your linking and you will see how much that control your in and out motion and how certain settings can hurt or help your process. 

 

20 hours ago, Aaron Eberhard - CNC Software said:

Yep, as Ron said, starting with X9, all of the multiaxis toolpaths became WCS aware...  That was my first release as the Product Owner *sniff* :)  Back when I trained you (X4?), it was REALLLY important to always have a multiaxis toolpath set in the Top WCS.

Basically, a plane is more or less irrelevant to a multiaxis toolpath (if you have one curve toolpath that starts on the front and then continues around on the side, what "plane" is that toolpath on?"), but the WCS is really important to us.   Changing from T/T/T to T/F/F will only change the way the data is stored in the background NCI (if you care, it goes from saving it as XYZIJK to XZYIKJ).  Because of the way you were digitizing on the machine at the time, the that plane inversion would alter the commanded positions of the probe, so on a digitizing Flow 5 Axis toolpath, it was REALLLY important make sure it was in Top/Top/Top before posting.

So the important thing to remember nowadays is that whenever you interact with an X,Y,Z in a multiaxis toolpath (Lock to 4 axis and rotate around Y, Limit the XZ plane motion, Fixed Angle to X, Retract Along Z, etc.), all of those X Y Zs are relative to whatever WCS the toolpath is in. 

I truly am not trying to be rude or obtuse, but I don't understand what y'all are saying here. It seems like you are speaking in a shorthand language, that you guys certainly know, buy I, sadly do not. 😢.

 

Share this post


Link to post
Share on other sites
52 minutes ago, So not a Guru said:

 

I truly am not trying to be rude or obtuse, but I don't understand what y'all are saying here. It seems like you are speaking in a shorthand language, that you guys certainly know, buy I, sadly do not. 😢.

 

No problem, I intermixed the current state of Mastercam with things that directly affected Motor-Vater, since I had originally trained him in Mastercam back in the X4 days, and a lot of what was necessary then doesn't apply anymore...

The main gist of the conversation was whether it mattered with a multiaxis toolpath to have all of your planes set to Top/Top/Top (abbreviated as T/T/T), because Motor-Vater was surprised to see that it worked fine to output it as Top/Front/Front or any other combination of Top/Xxx/Xxx.

So in Ron's reply and my first line, I was confirming that before the Mastercam X9 release, it was VERY important that you always used the Top WCS with a multiaxis toolpath (the planes didn't really matter for most people except in very explicit situations like I talked about with Motor-Vater in my second paragraph).   However, since X9, you've been able to use WCS appropriately with the multiaxis toolpaths.   As an example, a lot of people get a part in aircraft-coordinate-system, so when they load the part into Mastercam, it may be many meters away from the the T/T/T 0 point.   Previous to X9, you would have problems if you didn't move the part back to T/T/T 0, but after that, you can just create another WCS like you would for 3 axis work and it'll work perfectly fine.

My second paragraph was about what's happening in the background when you chance a toolpath from T/T/T to T/F/F behind the scenes and why it specifically applied to what Motor-Vater was doing back in 2009 or so and how it doesn't matter to most people most of the time.

The last bit was some general guidance on what you're doing if you set a multiaxis toolpath in a non-Top WCS, like my aircaft-coordinate-system example above.  When you choose the new WCS, all of the axis references (X,Yz) inside of a multiaxis toolpath mean "The X of chosen WCS"  NOT "The X of Top" like it used to before X9.

 

Does that help?

Share this post


Link to post
Share on other sites
50 minutes ago, Aaron Eberhard - CNC Software said:

So in Ron's reply and my first line, I was confirming that before the Mastercam X9 release, it was VERY important that you always used the Top WCS with a multiaxis toolpath (the planes didn't really matter for most people except in very explicit situations like I talked about with Motor-Vater in my second paragraph).   However, since X9, you've been able to use WCS appropriately with the multiaxis toolpaths.   As an example, a lot of people get a part in aircraft-coordinate-system, so when they load the part into Mastercam, it may be many meters away from the the T/T/T 0 point.   Previous to X9, you would have problems if you didn't move the part back to T/T/T 0, but after that, you can just create another WCS like you would for 3 axis work and it'll work perfectly fine.

Okay, that's what I meant to infer in my earlier response..

This is how understand it (and how I've always done my MC programming)

If I create a WCS, named PART_DATUM, that is not a derivative of Top. Any 5X paths must be programed in the "PART_DATUM / PART_DATUM / PART_DATUM" zero position.

That's correct isn't it?

Or am I allowed to program them in "PART_DATUM / a different construction plane / a different toolplane"? (which I've never attempted)

Share this post


Link to post
Share on other sites
23 minutes ago, So not a Guru said:

Or am I allowed to program them in "PART_DATUM / a different construction plane / a different toolplane"? (which I've never attempted)

Yes I do it all the time.

I will have a G54 Zero then I use create planes relative in the planes manager and get the planes I want relative to that and go from there. I may have G54-G59 base planes when I am programming a family of parts in one file.

Share this post


Link to post
Share on other sites
On 1/15/2020 at 12:48 PM, 5th Axis CGI said:

Not a big deal your post will do all the heavy lifting. Really comes down to how you need to define top? Does it need to be T/T/T or F/T/T? I have worked with many different configurations over the years and the post is what drives this not Mastercam anymore. 

In order to have the head at 0 and the table at 0 machining normal to X Y like a vertical machine. I would program from Top WCS/Right view for tool plane 

Share this post


Link to post
Share on other sites

I do enjoy when I open a can of worms... lol but seriously this is all good stuff to know. Mastercam has evolved in so many way over the years but some of us are such creatures of habit that we tend to not evolve with it. I myself always like to push the boundaries of what I am capable of, LOTS of times I look at something and know how I could path it, but will still take a trip down the rabbit hole in an attempt to get a better understanding of what I can accomplish and how. One thing I have learned over the years is mastercam is not very user intuitive, alot of paths can be made with a general understanding but the secret is to know exactly what u want to do and then trick mastercam into doing exactly that... 

Share this post


Link to post
Share on other sites
35 minutes ago, navsENG said:

In order to have the head at 0 and the table at 0 machining normal to X Y like a vertical machine. I would program from Top WCS/Right view for tool plane 

Then you already know the process to do what you need. Make a standard template folder with all your planes for this machine. Then import your file in that template. something I learned over the years is to keep a read only copy someone off the beaten path on your computer and network. You will accidentally overwrite the template many times before you train yourself not to. 

Share this post


Link to post
Share on other sites
22 minutes ago, motor-vater said:

I do enjoy when I open a can of worms... lol but seriously this is all good stuff to know. Mastercam has evolved in so many way over the years but some of us are such creatures of habit that we tend to not evolve with it. I myself always like to push the boundaries of what I am capable of, LOTS of times I look at something and know how I could path it, but will still take a trip down the rabbit hole in an attempt to get a better understanding of what I can accomplish and how. One thing I have learned over the years is mastercam is not very user intuitive, alot of paths can be made with a general understanding but the secret is to know exactly what u want to do and then trick mastercam into doing exactly that... 

Many different ways in Mastercam to accomplish a task and yes it does take going down many different rabbit holes, but the good thing is if you have gone down as many as I have you learn which ones are better and which ones are worse to go exploring in. 🤨

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us