Did you know Mastercam has "hidden" 5-axis toolpaths?

[slyym]

I get this error with triangular mesh toolpath??

 

Can't figure it out, and I've changed a million things

I did too. I messed with it until I changed the right thing and got it to work. Couldn't tell you what it was though. Just keep playin with it.

[daryl_y]

Hmmm.  I have seen the triangular mesh toolpath but never thought to give it a try.   The Module works toolpaths, parallel to muliple curves and morph between 2 curves I like and use a lot, These are also not just for 5 axis work and can be used in place of other surface toolpaths like parallel, flowline and blend.  Once you get past the initail settings (Mastercam really needs to figure out how to implement defualts on these) they are easy to use and give you a lot more control over the tool path. 

[Colin Gilchrist]

Sorry for anyone having problems. I'm not sure why you would be getting those errors. What kind of MD, and setup are you using? The ModuleWorks toolpaths seem to use the World Origin for some things. I'm not sure how good the support for WCS is, so you might have to move the model to the system origin, and try Top view for some things.

 

For those looking to try undercuts, the toolpath option you want is the "Geodesic". That one is designed to support undercutting toolpaths. I've been working on a new set of classes to cover the ModuleWorks toolpaths in the Multi-Axis module...

[Colin Gilchrist]

I think one of the best features of theses toolpaths is the control you get over the tool motion. I love the fact that you get two different "gap" settings. "Large Gaps" and "Small Gaps". That lets you use different options for different areas of the part, depending on how far the tool has to move between slices.

[Glenn Bouman]

Well this brings around a new topic. The last version of Mastercam with  a  bible attached (Mastercam Reference Guide)is what ?. Yes I am talking about that 831 paged thing last seen in X5. That is where you would think to find info like this.  But it seems we do not need one anymore , otherwise we'd have one. A teacher from a local college (newbie) asked how can he learn to use Mcam. I directed him towards the X5 doc .

 

it's like sex, you have to learn it on the streets )). Right now learning Mcam requires one to look in Youtube, Googling, etc. You'll find a tidbit here, tidbit there. 

 

Gracjan

 

I find this module works manual has a lot more info in it.

 

https://www.yousendit.com/download/elNJYUord0FTRTdFdzhUQw

[DRMutart]

didn work for me in X7......says 5 axis...contact reseller...asking for an access code.....

How is everyone else getting this to work????

[Rstewart]

didn work for me in X7......says 5 axis...contact reseller...

 

 

You obviously don't have the multi-axis license

[Rstewart]

I get this error with triangular mesh toolpath??

 

Can't figure it out, and I've changed a million things

 

 

Finally got the Adaptive roughing working and its pretty sweet!   Got a few quirks to work out but all in all it works really good!

 

What exactly controls the "Gap Settings" in the multiaxis paths?

[Colin Gilchrist]

Hi RStewart,

 

The Gap settings can be set under the "Linking" page, but it depends on which toolpath strategy you are using. The "Roughing" option doesn't let you define a Gap distance. It only lets you control the connection motion between "regions", "Slices", and "Groups".

 

I believe that these areas on the part are "automagically" determined based on how the toolpath itself identifies a group or region.

 

There are four Link settings that change the way the toolpath motion is calculated:

 

Within group = This is the option that controls the link between each cut of a pocket. (Green Link)

 

Between groups = This link controls motion moving from one "group" to another, within a pocket region (Purple Link)

 

Links between Slices = controls how the tool moves from one "depth cut" to the next. (Yellow Link)

 

Links between Regions = movement from one "pocket" area, to the next "Pocket" area (Red Link)

 

 

 

Here is a picture showing the Linking settings when "Parallel Cuts" is the strategy picked. You can see the Gap settings are now enabled. Once of my favorite things about the ModuleWorks toolpaths is that they let you define "small gaps" and "large gaps", instead of just having a single Gap size option.

 

 

 

[ChipBreakin]

Glenn,

      I tried to download that file from yousendit.com.  When I open it all I get is the dropdowns on the left side, nothing in the right window.  Is there a special program I need to open it with?

[Rstewart]

Thanks Colin!!

 

 I'll play around with those settings tomorrow when I'm not too busy.

[Guest MTB Technical Services]

Glenn,

      I tried to download that file from yousendit.com.  When I open it all I get is the dropdowns on the left side, nothing in the right window.  Is there a special program I need to open it with?

 

Go to the properties of the file and unblock it.

It's a MS security setting for handling compiled Help Files.

[ChipBreakin]

Thanks Glenn.  That was too easy.  Lots of good info in there.

[cobra95kev]

I have a question for the adaptive/triangular mesh gurus, I am trying this toolpath for the first time in X8 and I am running in to a problem with the roughing and adaptive cuts turned on using the climb and conventional option turned on it is giving me a feedrate on the conventional cut of 39.37 IPM and I am not sure where that feedrate is coming from, I see no option anywhere to change it? Is it a bug?

 

Edit: I did also download the help file linked earlier in this thread and was not able to find an answer in there.

 

Thanks,

Kevin C. 

[Müřlıń®]

Hello Everyone,

 

If you own a seat of Multi-Axis in Mastercam, you have a ton of great toolpaths that are available from ModuleWorks. There are actually a bunch of really great 3 Axis Toolpaths produced by ModuleWorks that are included in Mastercam, but they are almost "hidden" from the normal user.

 

These toolpaths aren't actually hidden from the user. But the Mastercam interface makes them appear to be something they aren't, so the average user, even the average Multi-Axis user, doesn't know they exist.

 

If you have a seat of Multi-Axis, do the following:

 

With a Machine Group loaded, go to Toolpaths > Multi-Axis.

 

If prompted, enter a new program name.

 

In the Multi-Axis dialog box, select "Surface/Solid", then select "Triangular mesh".

 

The Triangular Mesh toolpaths are the best kept secret in Mastercam. They have been available since at least X5, so they have been in the last few versions of the software.

 

The term "Triangular Mesh" is perhaps what makes these toolpaths "hidden" from the average user. Typically you would think of a Triangular Mesh object as an STL file, or some other external reference. In terms of the ModuleWorks toolpaths however, Triangular Mesh takes on a new meaning. For most of the 5 Axis toolpaths, the normal direction of the surfaces being cut plays a crucial role in determining the tool axis orientation. With the "Triangular Mesh" toolpaths, the surfaces themselves are not used to orient the tool axis. For these toolpaths the surfaces are simply tessellated using a cut tolerance.

 

In a nutshell, this just means that the "Triangular Mesh" toolpaths are just "3D Rouging and Finishing" toolpaths that don't take their tool axis direction from the surfaces being cut. They just provide great 3 Axis toolpaths that in some ways duplicate functionality in Mastercam, and in other cases drastically improve upon the existing options.

 

Once you've selected "Triangular Mesh" for the toolpath type, go to the "Cut Pattern" page, and look at the drop-down menu for "Pattern". This is where you select the toolpath type, and there are a bunch of them!

 

Toolpaths:

 

Rough

Parallel Cuts

Project Curves

Constant Z

Constant Cusp

Flatlands

Geodesic

Projection

Rotary

 

So that is nine different toolpath types that are available to you if you select Triangular Mesh.

 

Try the "Rouging" option. Activate the checkbox for "Adaptive" roughing, and now the style is similar to "Dynamic". But wait, it gets better. Normally with Dynamic style motion, you are only allowed to cut climb or conventional. Ok, so if you climb cut only, the cutter has to move from the end of the cut, to the start of the next cut, and typically does a micro-lift at a high feedrate to get there.

 

With the Adaptive rouging from ModuleWorks, you can use "Zig-Zag" stepover. This then allows you to enter 4 parameters: Maximum Stepover, Desired Stepover, Climb stepover percentage, and conventional stepover percentage.

 

So you can easily take say 75% of the stepover value for climb milling, then take 25% of the stepover value for conventional. This allows the cutter to stay fully engaged during the roughing cut, and allows for even higher metal removal rates than a regular "Dynamic" or "Opti" style roughing path.

 

If you've got a license of Multi-Axis, check out Mastercam's best kept secret...

 

SAAAAWEEEEET!

[oneyankfan1]

Why cant we have the step over control in adaptive cuts implemented into opti core and opti area? I am having over engagment issues in that tool path, or better yet why cant we get mastercam to actually hold a constant engagement through the whole tool path? The dynamic stuff is awesome but it needs refined, imo. Does anyone know if there are over engagement issues with triangular mesh yet?

[CristiP]

I find this module works manual has a lot more info in it.

 

https://www.yousendit.com/download/elNJYUord0FTRTdFdzhUQw

 

How did you open this? I can't see the content : (

[Guest]

Search out a chm reader

[So not a Guru]

I have this tool axis control set to from point, but it seems to be ignoring the selected point. Am I doing something wrong, or is this broken?

TEST.mcx-9

[So not a Guru]

I have this tool axis control set to from point, but it seems to be ignoring the selected point. Am I doing something wrong, or is this broken?

Or is this path restricted to 3-axis? I have to select a named plane to get it to cut from the direction I want.

[AGreen5]

On 9/18/2014 at 6:20 AM, rickcact1 said:

Why are those toolpaths buried so deep that it would be almost impossible to find? How many more things are hidden? Maybe a CNC software tech will reply and offer an explanation.

I ran into a similar situation trying to cut an interrupted multi index thread in mill turn. 
 

apparently the curve edge spline isn’t recognized as an arc to output smooth arc moves, but if you thread mill and convert the toolpath to geometry (something I haven’t ever done) and do some other savanti bullxxxx to select part of the helix and then toolpath that, it will be a work around that allows thread milling less than entire g12.1 full 360 helix initial moves?  
 

I’m not skilled enough to know that method, but if they simply had a “end degrees” check box in thread milling, it would allow the same to be derived from start and end degrees as if Mastercam wanted the user to derive function from the tool. 
 

these may be the issues making it difficult to staff Mastercam positions with qualified applicants at my company.   We need some jenie when applicants are just people with eyes and a brain like me trying to use the software as if it was setup to help a customer succeed.   
 

hooks are also weird to me, like someone at Mastercam is treating software like an old video game with cheats and hacks squirreled away for people who play video games in Monaco.  Hiding functionality or deriving it from an unusual number of extra operations is counterproductive. 

[Guest]

16 minutes ago, AGreen5 said:

hooks are also weird to me, like someone at Mastercam is treating software like an old video game with cheats and hacks squirreled away for people who play video games in Monaco.  Hiding functionality or deriving it from an unusual number of extra operations is counterproductive. 

Hooks are add-ons generally created by third party companies or individuals or companies, such as the verisurf tools and x+. Without hooks we wouldn't have those awesome tools..

It is also a great way to compartmentalize a program as any issues within a hook are restricted to that specific add-on making it easier to isolate and troubleshoot issues.

Creating programs in a modular fashion is a good thing imo. There is a lot to learn in mastercam, having good training resources and a knowledge base is important for a company.

Where I work, if there are complicated workflows I make screen recordings to serve as tutorials to newbies, since every companies workflow is different, I think that might help your situation.

26 minutes ago, AGreen5 said:

apparently the curve edge spline isn’t recognized as an arc to output smooth arc moves, but if you thread mill and convert the toolpath to geometry (something I haven’t ever done) and do some other savanti bullxxxx to select part of the helix and then toolpath that, it will be a work around that allows thread milling less than entire g12.1 full 360 helix initial moves?  

Can you post a Mastercam file demonstrating this? I would like to see what you are talking about.

[JParis]

18 minutes ago, AGreen5 said:

hooks are also weird to me, like someone at Mastercam is treating software like an old video game with cheats and hacks squirreled away for people who play video games in Monaco.  Hiding functionality or deriving it from an unusual number of extra operations is counterproductive. 

In addressing chooks...chooks are small applications, that particularly early on were used to created functionality and see if it was used and necessary. Many early chooks actually migrated to full blown Mastercam functions  and along the way, some little used functions or functions that have been made not necessary have been demoted to chooks...The coons chook is probably the most recent to be down graded...Netsurface has replace m uch of it's function...but it remains because there are those of us who still use it as in some cases it simply creates a better surface in some applications. The chook ability also provides a manner for people who want to develop their own hooks, for mostly their own use have an easy way in...there are other ways as well...chooks do have their place.

I think you need to remember, there isn't anyone who knows this software in & out....there are more than a few of us on this forum that have been with the software since V3(abt 1990/1991) of those, many know much more about the software but we then/we/I will tell you there are still things to be learned...

Over the years I have used other "high end" software and some of it I found to be incredibly powerful but so technical and difficult to use I have continued to this day to turn down ridiculous offers to program in that software.....they simply cannot pay me enough for the headache...

I know you're fairly recent to the software believe me though, I have never, in all my years, been given a part that if it could be made, was not able to accomplish it within Mastercam..

Show up and cut it

[cncappsjames]

To add to JP's comment, I'm one of those guys that has been using it pretty steady since 1992. I also have PowerMill, InventorHSM and Fusion360. Probably 80% of the time Mastercam is still my go-to CAM system, and probably 5% it's still my go-to CAD system.

 

There are certain things Mastercam just excels at and that's the bottom line. There's a few High-End things it excels at too. For allmit's quirks, lack of eye-candy, and lack of flash, it still gets the job done after all these years.

What does the future hold for the CAD/CAM industry? That is anybody's guess, but what I do know is the reality is that the the eye-candy, YouTube, and there's an app for that generation is in the driver's seat. They will be dictating how us Dinosaurs get our work done from here on out.

[AGreen5]

On 5/24/2020 at 7:30 AM, content creator said:

Hooks are add-ons generally created by third party companies or individuals or companies, such as the verisurf tools and x+. Without hooks we wouldn't have those awesome tools..

It is also a great way to compartmentalize a program as any issues within a hook are restricted to that specific add-on making it easier to isolate and troubleshoot issues.

Creating programs in a modular fashion is a good thing imo. There is a lot to learn in mastercam, having good training resources and a knowledge base is important for a company.

Where I work, if there are complicated workflows I make screen recordings to serve as tutorials to newbies, since every companies workflow is different, I think that might help your situation.

Can you post a Mastercam file demonstrating this? I would like to see what you are talking about.

I'm submitting a patent on the part I had to do ridiculous crap to post.  It's not conventional but also not that crazy of a part, but it's not been done in my industry before.  I probably should wait to submit it and re-visit it later.