Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

MP Master Post


Recommended Posts

Hi guys when using the MP Master Horizontal post is there a way to get the z axis to home before each B axis rotation?

Like when I use my 5-axis posts the Z axis will retract to home position before a 3+2 move.

Also what does the Misc Integer # 4 (Safe Index) do?

Thank you.

Misc.jpg

Link to comment
Share on other sites
On 8/31/2022 at 3:58 AM, Leon82 said:

I believe it does exactly what you want.

 

you can scroll thru the top of the post and it should have a description where they are declared

I have tried the Integer #4 on and off but when I ran machine sim the machine crashes when going from B0 to B90.

 

Link to comment
Share on other sites

try putting a 1 on this line

safe_index   : 0    #Currently hooked up to misc int 4

I think this is what you are looking for

ret_on_indx : 1     #Machine home retract on rotary index moves, (0 = no, 1 = yes)

 

make sure it's set to one

Safe Index forces a Z retract before X and Y motion

Link to comment
Share on other sites
12 hours ago, DavidB said:

I have tried the Integer #4 on and off but when I ran machine sim the machine crashes when going from B0 to B90.

 

Machinesim doesn't respect these switches unless you have purchased a Machinesim tied to a post. False Flag here what does the code look like?

Link to comment
Share on other sites
On 9/7/2022 at 10:41 PM, crazy^millman said:

Machinesim doesn't respect these switches unless you have purchased a Machinesim tied to a post. False Flag here what does the code look like?

The code is good it has a G28 Z0, Before the B axis rotation.

G00 Z165.833
G91 G28 Z0.
G00 G90 B90.
X148.5 Y542.861

How do I get the machine Sim to read the Z Home move?

 

 

Machine sim.jpg

Link to comment
Share on other sites
6 hours ago, DavidB said:

The Machine Sim reads the G91 G28 Z0. at the end of NC file but not during cutting.

G91 G28 Z0. (DOES NOT WORK)
G00 G90 B90.
X148.5 Y542.861

.

.

.

M05
G91 G28 Z0. (THIS WORKS)
G28 Y0. B0.
G90
M30
%

What we have been saying. Machine sim by itself is not good for situations like this or transform operations. With a Post tied to it then much better, but when you get into transform operation all bets are off.

  • Like 1
Link to comment
Share on other sites

As most of the work I do is HMC work and as I've learned, you gotta pick what you want to see....

My post is setup to automagically output a safe Z retract dendending on certain settings....as such and like you, MachSim does not pick it up without tying into the post($$$)

So my concerns are mainly working down and around the parts, that's my largest concern area, I KNOW it's going to retract....so I ignore that part and to get around it, I use exagerated clearance heights to get MachSim to see the jumps....

This allows me to get through and be reasonably confident that I'm not crashing into a part or fixture....current part I am programming is at this point 521 OP's, of those, about 100 are transforms....so I rely on transform HEAVILY..

I am hoping in 2023 to add real CAV software

Link to comment
Share on other sites
32 minutes ago, JParis said:

As most of the work I do is HMC work and as I've learned, you gotta pick what you want to see....

My post is setup to automagically output a safe Z retract dendending on certain settings....as such and like you, MachSim does not pick it up without tying into the post($$$)

So my concerns are mainly working down and around the parts, that's my largest concern area, I KNOW it's going to retract....so I ignore that part and to get around it, I use exagerated clearance heights to get MachSim to see the jumps....

This allows me to get through and be reasonably confident that I'm not crashing into a part or fixture....current part I am programming is at this point 521 OP's, of those, about 100 are transforms....so I rely on transform HEAVILY..

I am hoping in 2023 to add real CAV software

After the latest things Autodesk has done I know of some customers getting away from CAMplete and heading into different CAV directions. Other long time customers being offered it are getting CAMplete with new machine purchases to post NC Cdoe, but will be using other CAV since they offer comparison of the NC code back to the machined models to check for excess and gouges that CAMplete doesn't offer. Do I expect a mass exodus of customers no, but CAMplete like other purchased AD companies isn't what is use to be.

  • Like 1
Link to comment
Share on other sites
8 hours ago, JParis said:

As most of the work I do is HMC work and as I've learned, you gotta pick what you want to see....

My post is setup to automagically output a safe Z retract dendending on certain settings....as such and like you, MachSim does not pick it up without tying into the post($$$)

So my concerns are mainly working down and around the parts, that's my largest concern area, I KNOW it's going to retract....so I ignore that part and to get around it, I use exagerated clearance heights to get MachSim to see the jumps....

This allows me to get through and be reasonably confident that I'm not crashing into a part or fixture....current part I am programming is at this point 521 OP's, of those, about 100 are transforms....so I rely on transform HEAVILY..

I am hoping in 2023 to add real CAV software

Do you use TOP WCS and Front T/C Plane for B0?

Do you leave your WCS at the Centre of rotation of the B-axis?

I just bought a Mori NHX 4000 with G68.2 so I can set my WCS anywhere.

Link to comment
Share on other sites
12 hours ago, DavidB said:

Do you use TOP WCS and Front T/C Plane for B0?

Do you leave your WCS at the Centre of rotation of the B-axis?

I just bought a Mori NHX 4000 with G68.2 so I can set my WCS anywhere.

I do...WCS Top and planes wherever I need them...we don't have G68.2 on the HMC's....on our 5 axis machines, we have G68.2 and I do use that on those

I'm not sure I would use it on the HMC's even if I had it on them, unless something really required it for best use....I don't do any real 4 axis simultaneous cutting them. We could, just have had the need.

 

Link to comment
Share on other sites
  • 2 weeks later...

Correct me if I'm wrong but say I set my WCS to Center of the pallet rotation and I face the part as it sits in Mastercam. Say it might be Z350.

Then if the Billet was a little short in its height and the billet did not face, wouldn't I have to re-program everything again in Mastercam?

My concern is second OP's where I might have to set a WCS off a machined feature from OP1.

My Other Question is to Get B0 are you using Front or Top T/C Plane?

Thank you.

Link to comment
Share on other sites
On 9/17/2022 at 3:41 AM, JParis said:

I do...WCS Top and planes wherever I need them...we don't have G68.2 on the HMC's....on our 5 axis machines, we have G68.2 and I do use that on those

I'm not sure I would use it on the HMC's even if I had it on them, unless something really required it for best use....I don't do any real 4 axis simultaneous cutting them. We could, just have had the need.

G68.2 in an HMC is a great option. Should just be standard IMNSHO. What it does for you is makes it so you don't have to program from center of rotation or use multiple offsets any more if you have side work.

A difference between G68.2 and G54.2 is G54.2 requires you to either put your center of rotation X and Z (on an HMC) into either your Common Offset or your Work Offset and the distance from COR to your part origin goes into your G54.2 Offset Table (which you only have 7... or maybe it's 8.... hmmmmmm. I forget. It's either 7 or 8). With G68.2 you put your COR in parameters and pick up your offset(s if you've got multiple parts each with a different offset) wherever you want and it tracks.

Link to comment
Share on other sites
On 9/30/2022 at 9:08 PM, DavidB said:

Correct me if I'm wrong but say I set my WCS to Center of the pallet rotation and I face the part as it sits in Mastercam. Say it might be Z350.

Then if the Billet was a little short in its height and the billet did not face, wouldn't I have to re-program everything again in Mastercam?

My concern is second OP's where I might have to set a WCS off a machined feature from OP1.

My Other Question is to Get B0 are you using Front or Top T/C Plane?

Thank you.

To answer your question more dorectly, no, you do not need to reprogram....

Your WCS is TOP, it stays TOP but your T & C planes are reflective of your actual part origin....so that all you would need to adjust is your G5? of G54.1P?

 

Link to comment
Share on other sites

So WCS stays Center of Rotation but you can then set a Top T/C Plane on the part?

How is this Handled on the Machine?

It's been a long time since I ran and programmed for a Horizontal and I have a new Mori NHX arriving next month.

The centre of pallet rotation would be hard wired into the machine is that G54?

Then if I set a T/C plane on the part what would the G5? be in the posted code?

Any chance you could send me a Horizontal file to see how you go about it?

Thank you

Link to comment
Share on other sites
15 hours ago, DavidB said:

So WCS stays Center of Rotation but you can then set a Top T/C Plane on the part?

How is this Handled on the Machine?

It's been a long time since I ran and programmed for a Horizontal and I have a new Mori NHX arriving next month.

The centre of pallet rotation would be hard wired into the machine is that G54?

Then if I set a T/C plane on the part what would the G5? be in the posted code?

Any chance you could send me a Horizontal file to see how you go about it?

Thank you

 

Yes, the WCS is ALWAYS Top.....The T&C planes are origins where ever you want them....

The machine parameters "know" where the COR of rotation is, in this case, that doe not need to be accounted for...as it's already in the machine.

Yes, when you set your T&C place, you have an "origin" established at the point...you can choose which G54/G54.1P?? whatever..

My post automagically output all G5* origin locations, they get set via a G10 line...

I sent you a message, shoot me your email, I'll send over a sample file of how "I" do it... 

Link to comment
Share on other sites

Here you go David...

https://www.dropbox.com/s/veibgjwn3u6wpze/tombstone%20sample.mcam?dl=0

Now, the 99998888 is a raw posted file but you can see the offsets have output with a "basic" note on the origins...if you look inside of the 653 file, you can see how it looks after I clean it all up and get it ready for the machines.

Perhaps a couple caveats that won't fit what you're specifically planning on doing....

When it comes to our HMC's almost every single job a I program is a production job, the quantities are into the thousands and many run for several years, if not longer. We have parts running still that were orignially done in 2010, some sooner, On those, we set up at the begining of the years with 100,000 parts schehuled...many times later in the year we have to added a couple 10,000's to our yearly numners.

Consider when I came here, every program was output in incremental, every single offset have to be picked up by hand.....programs were created to run one part, once proven, the program came back into programming to have all of the transforms done, subprograms we non-existant....and then re-sent to the machine to be proven again and then signed off by QC. Desptie attempts, there was "no" standards....tombstone sizes with guesstimated, Y offsets were given off the top of the tombstone, all tombstone were aluminum and made in-house....there was a LOT of manual interdiction and work that HAD to be done to get a job running. Many times, it was a month or more.....

Now, programs are completly done ahead of time, I set all of those macro skips in it to allow running flexibilty. The setup guys and set it to run a single part and get that part signed off, they can then start tuening on faces and get those signed off.....ALL of the offsets are calculated in my post, and output as you see in the 99998888 file.

We've moved over to cast iron tombstones, every one we have purchased has gone into the machine within a .001" of centerline...we square them up just to "clean", they have a hard number to hit....if we are using hard tooling as in the sample file, those numbers are spot on...I just finished up a job, 4 sides, 8 parts on the upper section of the plate, 8 parts on the lower section of the tombstone....the upper section is Mitee Bites, the lower section is steel fixtures that in process parts can be mounted on to for machining. The guys running the show down there he hits the numbers I give him, this job was set to run a single part, it ran through clean with no adjustments to the offsets.....he turned on all 4 sides, not a single adjustment excpet for a diamter comp to hold a size and got the who tombstone signed off,...

If I were doing a single part, I would never use this method....but in a production area, setups have gone from a month+ sometimes where we can get through an entire setup, signed off and running in a couple days...and I mean to carve that time down even further.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...