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:

Mastercam 2022 Multi-Axis

#Rekd™

By #Rekd™,
in Industrial Forum

 Share

Recommended Posts

Metallic Newbie

Metallic

Posted
Posted

Oh boy this looks tasty! Half of my trouble with multiaxis is choosing the right method.

Im also glad they added the ability to manipulate the graphics window from within the toolpath parameters.

 

Im just guessing here that Mastercam is using and blending ModuleWorks packages to create this new "Unified" toolpath approach?

Link to comment
Share on other sites
Chally72 Collaborator

Chally72

Posted
Posted
17 hours ago, Metallic said:

Oh boy this looks tasty! Half of my trouble with multiaxis is choosing the right method.

Im also glad they added the ability to manipulate the graphics window from within the toolpath parameters.

 

Im just guessing here that Mastercam is using and blending ModuleWorks packages to create this new "Unified" toolpath approach?

As someone who constantly wants to iterate between morph/parallel on the same selection set, it is such a huge timesaver from just that aspect alone. Not having to match up several dozen subpage options/collision control choices to compare apples to apples cut pattern differences is really valuable.

Aaron would be the guy to ask about the latter question, but my understanding is that it's combining those Morph/Parallel/Along Curve packages in the background with our own special sauce added in to make it all a cohesive whole and open up some new possibilities.

  • Thanks 1
  • Like 2
Link to comment
Share on other sites
Aaron Eberhard Experienced

Aaron Eberhard

Posted
Posted
18 hours ago, Metallic said:

Oh boy this looks tasty! Half of my trouble with multiaxis is choosing the right method.

Im also glad they added the ability to manipulate the graphics window from within the toolpath parameters. 

 

Im just guessing here that Mastercam is using and blending ModuleWorks packages to create this new "Unified" toolpath approach?

Hope you like it :) I'm hooked, and I have trouble going back... But I'm biased!

 

You're correct, this is all MW tech running this, but it is a Mastercam-only creation.  I designed it and we created it just for our use.  It's really a big decision tree in the background that chooses the engine based on your input choices.

You're not only getting access to not only the surface-based technology you're used to (Morph, Parallel, Along Curve, Project Curve, and now Flow), but also a Geodesic-based algorithm, which is what gives us automatic boundary-based patterns, N guide curve input, etc.   There's a bit more magic happening of course, like if you have two curves selected and have it set to Guide, you'll get a Morph-style geodesic calculation and such. 

The real goal was that you feel free to just toss input in and you'll get a good toolpath out.   We have a few more tricks up our sleeve for the future, but I'm really, really happy with how it came out.

 

  • Thanks 3
  • Like 6
Link to comment
Share on other sites
gcode Experienced

gcode

Posted
Posted
8 hours ago, 1057880454 said:

Ask everyone, where can I download MasterCAM 2022 beat

I am not an official website member

I see that 2022 has a multi axis update, which is a great feature
 

Mastercam.com

you have to register to gain access

and you must have a valid Mastercam license installed on the computer you use to register

  • Thanks 1
Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
1 hour ago, huskermcdoogle said:

Last I had checked they wouldn't output in the old school paths either.....  did they at least hook that back up?

CAMPLETE will use it and a Custom post will also, but nothing Generic supports them. I had a switch added to support them before for the Moduelworks toolpaths and worked like a champ.

Link to comment
Share on other sites
huskermcdoogle Explorer

huskermcdoogle

Posted
Posted
17 minutes ago, crazy^millman said:

I had a switch added to support them before for the Moduelworks toolpaths and worked like a champ.

Yeah, I had a misc int for it in the past.  But given some issues with it on the machine I ended up not supporting it further in the future, I found it best to create a repeatable process and change cutters when they went out of spec.  But we were cutting wood so tool life wasn't an issue.  Typically speaking in half years or more....  It wasn't a problem for me to use comp, but it snagged the operators too many times, as sometimes it wouldn't take a 0 value.  Due to some parameter/toolpath issue I couldn't figure out, I for some reason couldn't convince them that a .001mm value wasn't going to effect things enough to worry about it.... Some vector/lookahead error on point to point cuts. 

Link to comment
Share on other sites
cncappsjames Experienced

cncappsjames

Posted
Posted
5 hours ago, huskermcdoogle said:

Last I had checked they wouldn't output in the old school paths either.....  did they at least hook that back up?

Old School Flow 5-Ax, Old School Curve 5-Axis and Old Scho Swart give you comp options. I use CAMplete exclusively for posting and it outputs G41.2/G42.2 just fine. This is why I don't use MW in Mastercam for anything but roughing 5-Axis. MW paths in MC don't have the tools I need to do my job.

  • Like 2
Link to comment
Share on other sites
Aaron Eberhard Experienced

Aaron Eberhard

Posted
Posted
13 hours ago, cncappsjames said:

Old School Flow 5-Ax, Old School Curve 5-Axis and Old Scho Swart give you comp options. I use CAMplete exclusively for posting and it outputs G41.2/G42.2 just fine. This is why I don't use MW in Mastercam for anything but roughing 5-Axis. MW paths in MC don't have the tools I need to do my job. 

You need to tell your post to output them, but we've had all of the same information available to the post for years now.  Any (CNC or MW) multiaxis toolpath that deals with surfaces will output the tool center point, tool vector, surface contact point, surface normal at the contact point, and all of the contour flags are accurate.

Edit: I just checked because I was curious, we added that for the 2018 release.

  • Like 2
Link to comment
Share on other sites
Guest

Guest

Posted
Posted
11 minutes ago, Aaron Eberhard - CNC Software said:

You need to tell your post to output them, but we've had all of the same information available to the post for years now.  Any (CNC or MW) multiaxis toolpath that deals with surfaces will output the tool center point, tool vector, surface contact point, surface normal at the contact point, and all of the contour flags are accurate.

Edit: I just checked because I was curious, we added that for the 2018 release.

So posts made in 2018 and before would need to be upgraded to support 5 axis comp?

Link to comment
Share on other sites
Aaron Eberhard Experienced

Aaron Eberhard

Posted
Posted
Just now, Thee Byte™ said:

So posts made in 2018 and before would need to be upgraded to support 5 axis comp? 

Edit:  Looks like Dylan beat me to it (I got a call before I finished responding so I didn't see his post).

 

Correct.

If you look at a simple toolpath like this morph:

image.png.a604e5e7dff7a4beec905723316ac5d3.png

The NCI looks like this:
  

G11       91.8510579 15.045 0.14187486 91.8510579 15.045 6.14187486 120. 20 0 -0.74213389 0. 0.67025166 96.30386121 15.045 2.12036487

You may already know this, but Posts are designed that they will ignore anything tacked on past whatever they care about, so if you drag a V9 post up through updates, it will still look at this part:
  

G11       91.8510579 15.045 0.14187486 91.8510579 15.045 6.14187486 120. 20 0

But it will just simply ignore the bits at the end (that tell it the tool contact position and surface normal vector): 

-0.74213389 0. 0.67025166 96.30386121 15.045 2.12036487

 

  • Like 2
Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
22 hours ago, Aaron Eberhard - CNC Software said:

You need to tell your post to output them, but we've had all of the same information available to the post for years now.  Any (CNC or MW) multiaxis toolpath that deals with surfaces will output the tool center point, tool vector, surface contact point, surface normal at the contact point, and all of the contour flags are accurate.

Edit: I just checked because I was curious, we added that for the 2018 release.

Then CAMPLETE is not supporting them correctly? Does someone from CNC need to reach out to them or does a end user/customer have to push CAMplete to get this supported since it has been available since 2018 and not implemented on their end?

What Generic Post from CNC Software supports them? How do we make MT output the code for them?

Link to comment
Share on other sites
cncappsjames Experienced

cncappsjames

Posted
Posted
25 minutes ago, crazy^millman said:

Then CAMPLETE is not supporting them correctly? Does someone from CNC needs to reach out to them or does a end user/customer have to push CAMplete to get this supported since it has been available since 2018 and not implemented on their end?

What Generic Post from CNC Software support them? How do we make MT output the code for them?

In the Mastercam File I/O settings in CAMplete I can totally specify comp supported toolpaths, however In MC's MW operations I don't see the pull down to set L/R/Control/Wear, etc... unless it's just automatic, which is kind of not optimal IMHO.

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
1 hour ago, cncappsjames said:

In the Mastercam File I/O settings in CAMplete I can totally specify comp supported toolpaths, however In MC's MW operations I don't see the pull down to set L/R/Control/Wear, etc... unless it's just automatic, which is kind of not optimal IMHO.

Kind of why I asked the question. I agree does us no good to get output if we have no way in the dialogs to tell the system what is the supported method in which we are planning on using it. It is kind of like I have 20 gear transmission, but only have the gear shift setup to go to 6th gear.

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...