Mastercam needs to fix...

[Bob W.]

I sure hope CNC fixes the issue of disappearing tools when multiple machine groups are used in a file. When I have a part that requires 5-axis and 3-axis machining in different setups I set up multiple machines in the operations manager. When I do this my unused tools disappear from my libraries. I also get several duplicate tools in my libraries. This has been going on for several releases and it is just pathetic.

 

I would also like CNC to fix the coordinate system issues with STL files. In the same scenario as above I will save STL files of the verify results and use them in another machine group for rest milling. Mastercam seems to screw up the orientation of the STL, which in turn screws up the rest mill calculations. They either need to clean up the process of creating the STL and which coordinate system is being referenced, or they need to allow the user to specify which one to reference.

 

I am frustrated right now because I have just sat here for three tries at rest milling an extremely complex part only to have the results come back as crap because the STL was not oriented correctly. It has been a few hours...

 

These two items only seem to be an issue when multiple machine groups are used in the same file. In my case it is a 3-axis mill and a 5-axis mill.

[Bob W.]

It is great that they are trying to develop new technologies and such but other aspects of Mastercam are just plain amateur hour.

[Verndog]

quote:

---

I would also like CNC to fix the coordinate system issues with STL files.

---

I believe they did this to interface with Vericut more seemlessly. It will 3d translate the STL to the WCS top you have selected (to top in new WCS). Simply go into WCS top / construction top to save your STL's and problem solved.

 

Also dont forget to set your stock view (stock setup tab) to top on the new machine group or your files will not verify correctly either.

[peon]

FIX THE VERIFY!

CREATE BETTER .STL FILES!

 

Large files using verify and Mastercam generated .stl files are KILLING ME!!

[Joe788]

Not that this is the right solution, but if you're using stl files of the verified stock already, why not just do the different machine ops as completely separate files? This would save a lot of your aggravation.

[Verndog]

quote:

---

Not that this is the right solution, but if you're using stl files of the verified stock already, why not just do the different machine ops as completely separate files? This would save a lot of your aggravation.

---

IMO this is the most painless method for large parts with multiple machine groups. With different machine groups the op manager jumps from one to the next in verify, kicks the screen view to some unknown view, messes with tool manager and dupe tools, forces WCS on 5 ax paths when some will not generate correctly with WCS and a handful of other issues. Also file size with all tooling for all ops, WCS getting busy, level manager now has to get scrolled thru...all those problems go away when you seperate op and file the part. Yes, I know they didn't design it to work this way, but the system works better with fewer issues because of all the work arounds and stalls from large file size.

[peon]

I have a 116mb .stl created by the verify utility. I just reduced that file down to 31mb using a trial version of Magics. Why can't Mastercam do that??!! I often restmill using the .stl files as a true stock reference.

[Bob W.]

Joe, the problem with that is these files see frequent revisions and it would be a real pain to try and track everything through multiple mastercam files. It is enough of a PITA with one Mastercam file. Mastercam is designed to work with multiple machine groups, now they just need to make it actually do that well.

[Bob W.]

Verndog, I see how much goes on to make Mastercam work with multiple machine groups but compared to generating a 3-axis toolpath it is pretty simple. It would be easy to fix this so it works well but first it needs to be a priority. There must be some real spaghetti code in there or this would have been cleaned up a long time ago.

 

I still love how when I right click and drag to copy an operation, my toolbar setup pops up. It reminds me of turning on the right turn signal in my car and having the wipers come on instead. VERY GHETTO!

[Verndog]

quote:

---

Mastercam is designed to work with multiple machine groups, now they just need to make it actually do that well.

---

Your in a tough spot with revisions. As far as a long term game plan, how long has X been out? That is how long the WCS and Machine groups and op manager have not played well together. Don't hold your breath to work as "intended" anytime soon. CYA since MC is WIP.

[Tim Johnson]

quote:

---

I sure hope CNC fixes the issue of disappearing tools when multiple machine groups are used in a file. When I have a part that requires 5-axis and 3-axis machining in different setups I set up multiple machines in the operations manager. When I do this my unused tools disappear from my libraries. I also get several duplicate tools in my libraries. This has been going on for several releases and it is just pathetic.

---

This is bug number cnc00063417. I sent this off on 09/25/2009.

 

When you open a file with multiple machine groups the unused tooling moves to the machine group that is holding the red arrow of doom.

[Bob W.]

So I should be finished programming this part but instead I am still trying to solve the issue and figure out how to rest rough this part. If I counted the hours that Mastercam crap like this wasted I would end up with a pretty big number. With CAM prices these days I will be looking at what else is out there whe it comes to adding another seat. I guess it is worth it to Mastercam to ignore crap like this but users are going to start moving on...

[Colin Gilchrist]

Peon,

 

With Magics you should be able to reduce that 116 MB file down to about 10 MB, with no appreciable loss of quality. If you have any questions about how to use Magics, email me through the board. I LOVE that piece of software.

 

For everyone else, try using the STL Heal Chook.

 

Also, if you aren't using any toolpath filtering, I highly suggest you start. Doing this will really help verify time, and will also reduce the amount of code you output. The only time I wouldn't filter a toolpath is if you have some kind of advanced contouring control that prefers to have lots of short toolpath segments. This is the one of the ONLY places the filter shouldn't be used.

 

I know it is a work-around, but on large files I will verify the part in stages. I only select 30-40 Ops at a time, and run them through verify. Then I save the STL, run STL Heal chook, and then load that healed STL file into Verify for more machining. I know it is a pain, but it really helps on larger files. I just got finished with a 150 Op part and this technique really helped.

 

Also, don't be afraid to open up your tool and STL tolerance a little bit, especially when roughing. One thing I constantly do is bump up the tolerances when I'm in the process of creating operations, say .004 and .004 for STL and Tool tolerance. Then after I've got all my operations pretty much finished, I'll do a final run through verify with my tolerances at .001 and .001. This really cuts down on my toolpath development time.

 

I'm really impressed with the improvements in X5 Beta for Verify. I'm seeing significant speed and quality improvements. I can't really say much more than that, but they are working on it.

 

One thing that will make a huge increase for ANYBODY who verifies large parts would be a Solid State Hard Drive. The read/write times on large parts will kill your verify speed.

[Colin Gilchrist]

Bob,

 

I use a method for STL production and verification where I never need to use the Xform STL function to get the file in the correct place.

 

I only use the system "Top" view for STL files. If the part starts in a WCS, then I create and use a Solid for the first Op. As long as you don't change your "Stock View" in Stock Setup, all your STL models will be correct and you can save them right out of Verify and then use them in your Rest Roughing Ops.

 

I know, I know, the Stock View should just work. It really needs improvement, and they are working on it.

 

If you do need to move an STL file, between Machine Groups for example, then I would use the Xform STL for moving it.

 

It takes some getting used too, but I swear by this method because your stock never gets lost between Ops, or when saving from the Verify module. It just works and that is the main reason I do it this way, because I don't have to constantly think about it. It has been 100% reliable for me since X2, and that is saying something...

[Colin Gilchrist]

One last thing for everyone:

 

If you use the Xform STL function, the default for the system is to only display 5000 triangles. On large parts this will often only show a small portion of your STL model.

 

On the Xform STL dialog box, there is a data entry field for "# Tris", this is the number of triangles to display. If you enter "0", Mastercam will display all the triangles and show the entire STL file...

[Tyler Robertson]

Your STL file will be created in the orientation of your CPLANE. When you save, make sure your CPLANE is the same as the orientation of your part.

Problem solved?

 

Would be nice to have a dialog to select the orienation, sure - but I don't think this is an 'amateur hour' problem.

 

What colin said as well - it makes sense, and if you just follow that procedure it won't get lost.

 

 

My question with the machine groups is why have two?

 

You can have a machine group for one machine and still do 3 axis or 5 axis work from one machine group

 

 

Again, I'm not 'excusing' - but I think you're getting too caught up in the problem without looking at a current solution.

[Zoober]

I have looked into Magics, did the demo, and Colin is 100% correct. It rocks!

But unfortunately, I couldn't get the mucky mucks to part with that much $$.

So instead, I went with VRMesh Studio. It is a fraction of the price, does much less tyhan Magics, but for accurate decimation (which really was all I needed for cutting down huge STL files) it is every bit as valuable as Magics.

I don't mean to step on your toes Colin, but I just wanted to point out a low cost solution to those that can't/won't afford Magics.

[peon]

Thanks for the suggestions Zoober and Colin. I doubt the higher-ups will let me purchase either of those packages. I'm just wondering why Mastercam can't create or fix an .stl that is usable on the larger files.

[peon]

Zoober, I just installed the trial version of VRMesh 5.0 Studio. What procedure do you use to reduce the triangles?

[Bob W.]

Tyler,

 

How would I do 3-axis and 5-axis work from one machine group? My 5-axis post will always post A and B positions even if the work is 3-axis. This will alarm my machine if it doesn't have the trunnion installed. I also have both machines set up with different tools and they both run simultaneously.

 

My frustration has grown over the years with all of these little issues. They are time wasters and it really adds up. CNC has known about them forever but it doesn't seem to be a priority for them to fix. Mastercam does seem pretty 'amateur hour' compared to the other professional software packages I use like Solidworks or ProE. Here is a small list of my daily issues...

 

The verify crashes regularly, it doesn't handle large files well

 

I get prompted to select the color of entities when opening Mastercam

 

The toolbar config window pops up when copying operations

 

Tools disappear and get duplicated when having multiple machine groups in one file

 

Unhandled Exception...

 

I could go on and on. These aren't new bugs, they have been around for years now. Would you deliver parts or posts with this many bugs or issues after your 15th try?

[Zoober]

Peon, import the STL file

On the Modify menu, select Decimation

In the tool box on the upper right, I use (checked box):

Quadratic

Preserve Boundary

Preserve Marked

Percentage

On the Percentage slider, I start at 66%

Apply to Selected object

 

Now, hit apply, and look to the status bar lower left to see completion.

Now, export to a file. I just use the same and let it overwrite original. I have never had problems doing that, but you may want to specify a different file name to be careful.

 

Let me know if you need more.

[peon]

Hmm, those settings increased the file size by another 32mb. I'll have to keep playing with it.

[Tyler Robertson]

Sorry I was a little narrow minded - I set up posts differently and shouldn't expect your post to be like that.

[Zoober]

I don't know why it would, Decimation lowers the triangle count. I've never seen one increase yet..

If you can put it on the FTP, I can take a quick look.

[bhyde]

Sweet! I did not even think of using Magics for this purpose at all. Use it plenty for the SLA..Thanks guys!