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:

Matsuura MX520


Schuero
 Share

Recommended Posts

On 11/22/2021 at 2:14 AM, Schuero said:

Hello Everyone,

Dose anyone have experience with Hi Cut settings on matsuura machines,...?

Which Hi Cut do you use for OptiCore operations,...?

I have the problem that the machine is not running smoothly during the operation,..

I use G131 F3 as default,...

F3 is a high accuracy, multiaxis finishing setting.  I would guess F1 would do a whole lot better.

 

G131 P(1-3) - 2 axis machining

G131 M(1-3) - 3 axis or 3D machining

G131 F(1-3) - Simultaneous 4 or 5 axis machining

G131 D1 (only 1) - Drilling or Tapping

1 leaning towards speed/roughing, 3 leaning towards finishing/accuracy.  

 

Unless it's one of the older HandyMan types, then it's G131 R(1-10)

 

Anyone more knowledgable, feel free to correct me.

 

Link to comment
Share on other sites

There are 3 tables in the ipc settings.

You can fine tune each one. There is a column for 1 and for 10 the middles are extrapolated from the two.

On ours they are very similar. There is a slider for 1-3 4-6 and 7-10.

If you use p you are using where the slider is.

 

You can program r7 for non critical stuff then go to r 10 for a tight contour and back to r7 without having to move the slider.

Link to comment
Share on other sites
On 11/21/2021 at 11:14 PM, Schuero said:

Hello Everyone,

Dose anyone have experience with Hi Cut settings on matsuura machines,...?

Which Hi Cut do you use for OptiCore operations,...?

I have the problem that the machine is not running smoothly during the operation,..

I use G131 F3 as default,...

G131 has 4 different arguments;

1) P for 2-2 1/2D Prismatic type machining (2D HST, Contour, Pocket, Thread Mill, Circle Mill, Engraving, Chamfer, etc...)

2) M for Multi-Surface (High Speed Dynamic, 3D Surface Machining, etc...)

3) F for any rotary axis type cutting

4) D1 for Drilling/Canned Cycles

In P, M, and F's arguments there are 3 Settings;

G131 P1, G131 P2, and G131 P3

G131 M1, G131 M2, and G131 M3

G131 F1, G131 F2, and G131 F3

1 = Smoothness/Roughing Preference

2 = Semi-Finishing/Balanced Preference

3 = Finishing/Accuracy Preference

 

Within P, M, and F on the IPC settings page there are sliders. the 1 and 2 sliders have 3 slider positions, speed preference, balanced preference and accuracy preference, the 3 slider has 4 slider positions speed preference through accuracy preference with two settings in between.

 

I would expect G131 F3 to not run smoothly in the case you illustrated. I would recommend G131M1 with that tool path.

Do not use "3" as a default for anything other than what you need to hold mid-low single digit micron accuracy on.

 

Using the correct mode for the right tool path is the key to getting the desired machine performance.

  • Like 4
Link to comment
Share on other sites

You have to go to the mims or handyman or side panel button on the machine to see what you have

16 hours ago, SuperHoneyBadger said:

Are you referring to a page in the machine control here?

I'm mostly at the MC seat, so I don't get to poke the buttons on our VX660 too often, and I can't see where these settings would be in MasterCam

You can use a manual entry in mastercam or make post changes to use mic values or canned text

  • Thanks 1
Link to comment
Share on other sites
20 hours ago, SuperHoneyBadger said:

Are you referring to a page in the machine control here?

Correct. There is an IPC Settign page on the control. Currently this is the only way to fine tune the IPC settings. We've been asking Matsuura for the ability to control that through program input. So far, it's still in the suggestion box.

But in the program G131P/M/F/D1 ... that is driven by program/g-code.

  • Thanks 1
  • Like 3
Link to comment
Share on other sites
On 11/30/2021 at 3:25 PM, cncappsjames said:

2) M for Multi-Surface (High Speed Dynamic, 3D Surface Machining, etc...)

James, I've always used P for my dynamic milling, and opti-rough, and I was looking at them as 2d machining, as they're generally only moving in 2 axes at a time while making a cut.  Will I get better results using M for these toolpaths?  I also noticed in the other thread that was linked earlier in this thread, he mentioned using M3 on opti-rough toolpaths.  I would think you'd always be using a 1 with opti-rough.  Is there ever a reason to use a 2 or 3 when roughing?

Link to comment
Share on other sites
3 hours ago, JB7280 said:

James, I've always used P for my dynamic milling, and opti-rough, and I was looking at them as 2d machining, as they're generally only moving in 2 axes at a time while making a cut.  Will I get better results using M for these toolpaths?  I also noticed in the other thread that was linked earlier in this thread, he mentioned using M3 on opti-rough toolpaths.  I would think you'd always be using a 1 with opti-rough.  Is there ever a reason to use a 2 or 3 when roughing?

There's been some debate on the P vs. M for the dynamic stuff with no real definitive consensus. I'll be in a meeting with the Matsuura guys this morning. I'll ask if they have done any further testing.

I would NEVER "ROUGH" with a 3 regardless of the P, M, or F mode. That's just literally leaving money on the table. 3 is meant for like when you need to hold single digit micron accuracy on features. If somebody needs to hold single digit micron accuracy on a roughing op, I'd suggest a SERIOUS re-evaluation of the process. I can't come up with a scenario where I would ever rough with a 3.

  • Like 1
Link to comment
Share on other sites
1 hour ago, cncappsjames said:

There's been some debate on the P vs. M for the dynamic stuff with no real definitive consensus. I'll be in a meeting with the Matsuura guys this morning. I'll ask if they have done any further testing.

I would NEVER "ROUGH" with a 3 regardless of the P, M, or F mode. That's just literally leaving money on the table. 3 is meant for like when you need to hold single digit micron accuracy on features. If somebody needs to hold single digit micron accuracy on a roughing op, I'd suggest a SERIOUS re-evaluation of the process. I can't come up with a scenario where I would ever rough with a 3.

Sounds good.  I thought the roughing with a 3 seemed odd.  I've always used _1 and it works.

  • Like 1
Link to comment
Share on other sites
17 hours ago, cncappsjames said:

Depending on tolerances often times I'll even finish with a 1. No reason to run any tighter than necessary.

I've been using a 1 for most things, unless the tolerances are less than like 100µm.  Sometimes I'll play around with the accuracy level to improve a 3D toolpath.  

 

When I first started using this machine I ran an Opti-Rough toolpath with no IPC turned on at all.  A good sized corner of the part vanished when it made the first transition move.  😂🤣

  • Haha 1
Link to comment
Share on other sites
21 hours ago, cncappsjames said:

I always rough with 1.

Our post outputs this line:

G131 (HI-SPEED)

We have a misc. value called "Hi-Speed Style", and when it gets set to 1, the post adds the above code on it's own line after the toolchange, and carries on until it's cancelled (every op).

Is this naked G131 line the same as G131P1? I'm hoping it is, so I don't have to delve into the post, or even worse - add manual entries for the calls.

Link to comment
Share on other sites
5 hours ago, SuperHoneyBadger said:

Our post outputs this line:

G131 (HI-SPEED)

...

Is this naked G131 line the same as G131P1?

Negative ghost rider. G131 all by itself is equivalent to roughly the old High Speed Modes that use R-Values.

G131 by itself ... G131R8

So I take it you are not using CAMplete?

  • Thanks 1
Link to comment
Share on other sites
17 hours ago, cncappsjames said:

So I take it you are not using CAMplete?

That's a big 10-4.

I have MasterCam 2021 and 2022, that's the full kit I can bring to bear on my parts. I hear you guys throw around CAMplete, Verisurf and all those other fancy, book-learnin' programs all the time. I have been operating under the assumption that I am not skilled enough to know that I need them.

Without de-railing the thread totally, what is its purpose?

Link to comment
Share on other sites
1 hour ago, SuperHoneyBadger said:

That's a big 10-4.

I have MasterCam 2021 and 2022, that's the full kit I can bring to bear on my parts. I hear you guys throw around CAMplete, Verisurf and all those other fancy, book-learnin' programs all the time. I have been operating under the assumption that I am not skilled enough to know that I need them.

Without de-railing the thread totally, what is its purpose?

CAMPlete is a complete Posting and NC Code Verification engine CAV(Computer Aided Verification) in one. Currently with even the best post out of Mastercam tied to the Machine simulation you are not checking back to the posted NC code you are only checking the pre NC code called NCI for collisions and other things. The missing element in the Mastercam equation has always been control emulation where the verification is mimicking what a CNC Control does to check for possible errors or collisions that will be missed when programmed in the CAM said of things. With ICAM now coming under the same ownership as CG Tech and CNC software now maybe someone will happen with putting together a all in one process cradle to grave of the digital twin everyone keep claiming they have when in all reality the majority only have bits and pieces of it.

I am currently programming a Mill/Turn on the 6th revision the part. Crazy deep undercuts and other things got added in the last revision and I am having to change tool holders and all kind of things to make it fit in the machining envelope. Without CAV it would be days if not weeks of time on the machine seeing all the errors the CAM is not showing me. By using CAV I am able to digitally see the errors and make changes; then check for issues before they ever get to the machine. I did this 20+ years ago without CAV and got it done like you are currently doing, but with a CAV process I save time and reduce possible errors at the machine before they every get there. Nice to post a program and feel comfortable running it verse standing at the machine praying I thoughts of and caught everything. Without it you may have got your process dialed in so well you are comfortable doing that, but after doing this for 35 years I still am never 100% sure of any program I make until it has been run on the machine.

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
1 hour ago, SuperHoneyBadger said:

That's a big 10-4.

I have MasterCam 2021 and 2022, that's the full kit I can bring to bear on my parts. I hear you guys throw around CAMplete, Verisurf and all those other fancy, book-learnin' programs all the time. I have been operating under the assumption that I am not skilled enough to know that I need them.

Without de-railing the thread totally, what is its purpose?

CAMplete TruePath is Post Processing, Simulation, and Collision Checking software that comes standard with every 5-Axis Matsuura sold in the US. It does things even the best post processors on the planet can't do, or can't do easily. I've been using it since about 2006. Matter of fact, I think I only have one post from a Post Builder for one of our models and the only reason I have it is because I needed to do some testing for the customer.

CAM is only part of the machining puzzle. You can have the awesomest CAD/CAM software but if you don't have full featured posts, don't have a means for simulation/collision checking the code (at least on 5-Axis machine for sure), then there's a good chance something unforseen will pop up that could cost A LOT of money.

Back to High Speed Modes, I would suggest contacting your local Matsuura dealer and get them to come in and do some training with you. You're missing out on some key features of the machine/control. I'll add, you should get in contact with your Mastercam dealer as well and make sure there is provision for setting the proper High Speed Modes for the type of toolpath being used, and the proper level based on desired outcome.

  • Like 3
Link to comment
Share on other sites

As much as I love to hate on and bash Haas, they do a GREAT job of teaching their machine control features on Youtube.  I wish other machine tool builders would follow suit and put some instructional material out there.  I have Makinos and a DMG mill-turn and figuring this stuff out is brute force trial and error which sucks @ss.  It would take Matsuura, Mori, Makino a day or two to produce a 30 minute video that would go through the basics of this setting and the end result would be a much more productive customer AND an AE with more time to work on other things as well.  One time investment...  That is probably the last good thing I'll say about Haas for a while :-).  

What I have done with Mastercam is edit my post so I can set these parameters using the misc integers and/ or misc reals.  That way I can set them on an operation by operation basis with no hand editing.  I did that by trial and error but I am pretty comfortable tweaking my posts.  If you don't want to mess with your post I'm sure your reseller could modify it for a small fee.  It is time and money well spent.  Post and run with no edits, the ONLY way to fly.

Also, as others have mentioned, get simulation software before you scrap your machine.  I use Vericut but for Matsuura Camplete is the ticket.  I wouldn't even consider programming and running a 5-axis machine without simulation software (NC simulation software).  These machines are so damn fast there is no way an operator will catch everything unless running painfully slow and wasting a crapload of valuable machine capacity and spindle time.  You will ultimately pay for it one way or another...  It is kinda like getting a HSK100 box way machine and using ER collets to hold you end mills...

  • Like 2
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...