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:

Haas UMC 750

Masterminder408

By Masterminder408,
in Industrial Forum

 Share

Recommended Posts

Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Hello Mastermind,

 

Yes, you can certainly take the Generic Fanuc 5X Mill Post and edit it for the machine yourself. Like Ron mentioned we did work with Haas directly to make sure all the features of the machine are fully supported. There are some features like TCPC and DWO that take quite a bit of editing to get implemented correctly, but any savvy post writer can do that themselves.

 

Best regards,

 

Colin

Link to comment
Share on other sites
Masterminder408 Newbie

Masterminder408

Posted
  • Author
Posted

Masterminder did you get the machine yet?? Do you guys use and type of g-code verification with your 5 -axis machines? It might be our 1st 5 axis so Im looking for any tips I can get about what else We need to go with the machine.

 

Machine is on the way here, we do not have any g-code verification, only use mastercam simulator, mastercam does what it said so there is no need for a NC verification..., and having the post from CNC....we have couple of TR-210 here, used mastercam and it own verification and machine simulation and I have no problem with it....from very simple to very complicated stuff...

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Hi Bob,

 

Yes, the UMC-750 has those control options. I believe they are standard for this machine, but I could be wrong. The TCPC is only valid for 5 Axis machining, and the DWO is only valid for 3+2. That's what we've built into the OEM Haas UMC-750 Post Processor. It is also setup for High Speed codes and compatible with the Productivity+ Probing add-on. Each OEM post comes with a PDF 'Applications Guide' that explains how to use the post with Mastercam, and set all the switches properly. We've tried to make sure every feature on the machine is supported "out-of-the-box", and it also comes with a full model for Machine Simulation. The post is still technically in a Beta state, as we are still working through some tests with Haas corporate to get the post certified. Anyone interested in an OEM Post should talk with their Mastercam Reseller for more information.

 

Thanks,

 

Colin

Link to comment
Share on other sites
Newbeeee™ Community Regular

Newbeeee™

Posted
Posted

Each OEM post comes with a PDF 'Applications Guide' that explains how to use the post with Mastercam, and set all the switches properly. We've tried to make sure every feature on the machine is supported "out-of-the-box", and it also comes with a full model for Machine Simulation.

:respect:

Link to comment
Share on other sites
Masterminder408 Newbie

Masterminder408

Posted
  • Author
Posted

Hi Bob,

 

Yes, the UMC-750 has those control options. I believe they are standard for this machine, but I could be wrong. The TCPC is only valid for 5 Axis machining, and the DWO is only valid for 3+2. That's what we've built into the OEM Haas UMC-750 Post Processor. It is also setup for High Speed codes and compatible with the Productivity+ Probing add-on. Each OEM post comes with a PDF 'Applications Guide' that explains how to use the post with Mastercam, and set all the switches properly. We've tried to make sure every feature on the machine is supported "out-of-the-box", and it also comes with a full model for Machine Simulation. The post is still technically in a Beta state, as we are still working through some tests with Haas corporate to get the post certified. Anyone interested in an OEM Post should talk with their Mastercam Reseller for more information.

 

Thanks,

 

Colin

 

 

Colin,

 

TCPC and DWO is standar for UMC 750, I did talked with my reseller regarding OEM UMC 750 post, and yes we 're going to purchase it from CNC...thanks for the head up...

Link to comment
Share on other sites
MrFish Enthusiast

MrFish

Posted
Posted

Get Gcode verification of some sort . The first time you stack it on a re-postion move that wasn't simulated in the mastercam simulation because it was generated at the posting stage you will wish you had it. Especially if it is a decent stack that throws out the machines axis and wrecks a spindle, Gcode verification will seem like a cheap safety !!

Link to comment
Share on other sites
Bob W. Apprentice

Bob W.

Posted
Posted

Get Gcode verification of some sort . The first time you stack it on a re-postion move that wasn't simulated in the mastercam simulation because it was generated at the posting stage you will wish you had it. Especially if it is a decent stack that throws out the machines axis and wrecks a spindle, Gcode verification will seem like a cheap safety !!

 

Couldn't agree more. Also, I don't believe Mastercam will simulate TCPC or DWO in its machine simulation. I ran my Makino in 5-axis for about 10 minutes before I was on the phone ordering machine simulation from Vericut. It only took that long for me to realize I could buy it right then for $xx,xxx or I could buy it in 6-8 weeks for $xx,xxx plus the cost of a new Makino spindle and repairs to my Tsudakoma rotary table, which would be about triple the cost of the Vericut... I was pleasantly surprised at how much time it has saved me in addition to preventing crashes. It has been one of the best investments I have made for increasing my productivity in the shop and it was worth every penny. Buy it now or buy it later, especially if you will be running TCPC and DWO.

Link to comment
Share on other sites
Masterminder408 Newbie

Masterminder408

Posted
  • Author
Posted

Mastermind, What kind of tooling/vise setup are you going to be using with the umc-750? what kind of work do you guys do?

 

We will be using our own plate on top of it original plate, with re-enforce pin pattern, so that we can use almost every fixture that we have in our shop, everything is bolt down with 2x .500 pins and 4x 1/2-13 screws,,, I haven't purchase any work holding yet, and not planning on to.... saw a couple of work-holding but didn't like the method of it.. so everything is custom made in house...

 

 

Couldn't agree more. Also, I don't believe Mastercam will simulate TCPC or DWO in its machine simulation. I ran my Makino in 5-axis for about 10 minutes before I was on the phone ordering machine simulation from Vericut. It only took that long for me to realize I could buy it right then for $xx,xxx or I could buy it in 6-8 weeks for $xx,xxx plus the cost of a new Makino spindle and repairs to my Tsudakoma rotary table, which would be about triple the cost of the Vericut... I was pleasantly surprised at how much time it has saved me in addition to preventing crashes. It has been one of the best investments I have made for increasing my productivity in the shop and it was worth every penny. Buy it now or buy it later, especially if you will be running TCPC and DWO.

 

Thanks Bob, I did a webinar with vericut, and we 're considering it only for the 5-axis module...we do not use any other G-code verification in house other than Mastercam,... to me I think that 's enough, so far I have a lot of luck with it, and the simulation is great...

Link to comment
Share on other sites
Allan Newbie

Allan

Posted
Posted

Re: G Code verification

 

Has anyone ever considered:

 

Any computer program simulating G Code is not "Running" gcode, it is using an interpreter.

So it reads G Code and interprets that into motion and actions.

You would most likely find issues/limitations using with this "Running" G Code interpretation software (no matter the brand).

 

 

The Machine simulation in Mastercam can be driven from the post processor (the same one that makes the G Code), isn't that good enough?

Link to comment
Share on other sites
Bob W. Apprentice

Bob W.

Posted
Posted

The Machine simulation in Mastercam can be driven from the post processor (the same one that makes the G Code), isn't that good enough?

 

Okay, so if you set up your part on the machine to run DFO, or DWO, or TCPC will the Mastercam simulation show the crash that might ensue if the G10 lines are entered incorrectly? Can you input the part coordinates to accurately place it on the machine? Will it tell you the minimum tool gage length needed to prevent a crash? Will it give you the alarm if wear offset is activated in an arc move preventing a trip back to the computer to fix and repost the program? Will it accurately simulate the macros that are on the machine that are called during the course of machining (probing, gun drill, etc...)?

 

From what I have seen running Vericut the primary value is not in the crash prevention, which is what I bought it for. The real value is in the number of trips between the machine and computer it has saved me because it catches everything, not just collisions. I can adjust my tool lengths to fix over travel issues, catch all of the syntax issues such as wear activated on arc moves, catch pilot holes too small for taps (drilled for cutting tap instead of forming tap), etc... The amount of time it saves on those daily issues adds up big time. I can also load a program hit start, shut off the lights and walk out the door at night and get a good nights sleep knowing that it is bulletproof.

 

To be perfectly honest, I would not trust the reliability of Mastercam to get this right. Some of the issues I have seen over the years just make me scratch my head and I would not be able to sleep well at night knowing that machine sim said everything was good to go. Heck, I have tools going corrupt and disappearing from my Mastercam toolpath libraries every day and I am going to trust my $400k Makino to machine sim that uses this data? I don't think so. You are right though, it has to be set up correctly. GIGO applies to every aspect of computing and for me, the only thing I regret about Vericut is not buying it sooner. It has had a fantastic return in productivity. I don't care about the Mastercam tool library issues or advances anymore because Vericut handles all of that and it flat kills it! Same with reports and setup sheets.

Link to comment
Share on other sites
Newbeeee™ Community Regular

Newbeeee™

Posted
Posted

The Machine simulation in Mastercam can be driven from the post processor (the same one that makes the G Code), isn't that good enough?

Alan - is this a default or a setting?

 

I think it's always good practice to have a second opinion (as in independent verification).

We use NCPlot which is fantastic value for money (and can handle sub progs) but we only have 4axis verticals.

If I had 5axis, I wouldn't hesitate in getting vericut or the like.

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
Go to topic listing

  • 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.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...