fatal error in verify

[billet programmer]

using x4

 

When I try to save the result of verify as an stl file I get this message:

Fatal error occurred in verify/simulation

Please exit verify & try again with reduced image quality.

At this point it will not save.

 

Does anyone know how to get rid of this?

[Guest]

Have you tried running a larger tolerance on your stl resolution?

[Code_Breaker]

quote:

---

Have you tried running a larger tolerance on your stl resolution?

---

I have, three or four times a day, but when measuring, it is +/- your tolerance ... in many cases with me, I MUST have tighter tolerances ... ususally .001 ...

 

This only happen on larger files where the the STL are over 15MB ... very common here ... so I have to use Vericut for FINALLY verification ...

[billet programmer]

I have my stl tolerance set as .001 by default. I reset it to .005 and am running the verify now... I'll keep you posted. Thanks, John

[KMartin]

I'm having the same problem .Larger tolerance doesn’t help.

[Zoober]

I do a lot of restmilling, and have had STL's up to 800MB.

Generally, when I get that error, it is a lack of memory that a reboot (not just restarting MCX) will restore. I am not sure whether or not the leak is MCX, Windows, RAM, or Graphics, but if I do a lot of verifying, it seems to leak more, causing a more frequent reboot.

I used the Magics program (Colin can explain Magics better than I) to lower the triangle count, which helped greatly, but It was the trial version, and I don't think my Co. will pop for it, so I keep rebooting. As the STL gets larger, the problem gets more frequent.

Making the tolerances larger as JP says above helps to keep the file smaller.

Mine are set at .002 for both tool and STL.

I have had to go up to .008 for larger files to work.

[billet programmer]

I finally got it to work by setting my tool tol. to .005 and the stl tol. to .01

 

Thanks everybody.

[peon]

What good is the verify if you must loosen those tolerances?

[Guest]

What good is it if you're only bitchin peon.

 

This is a help forum.

 

We "helped" him get his job done.

 

Get it?

[peon]

Bitching? I just wanna make him aware that he may have eliminated the error, but is the final result on the steel correct? There is certainly a trade off! Billet, you may be fine with the increased tolerance, but if you are machining molds with very fine detail, please be aware that you will need to tighten them tolerances or use a third party verification software.

[Zoober]

As I said earlier, I work with pretty large STL files, and as such need to loosen my tolerances.

I have never had problems going to .008 as far as accuracy goes. You cannot rely solely on verify to ensure part accuracy. There are too many variables at the machine......

Rigidity, tool deflection, chip evacuation, etc..

 

I think it is better to ensure proper process than to rely on what verify gives me in return. If I have planned the job correctly, .008 difference in verify is not going to kill my rate of success. I am looking for stupid errors (on my part) that are going to cut the part in half, or render my fixture useless for the next part.

Shoot, a lot of guys I know don't even run STL compare anyway. If you need more accuracy feedback, you probably need Vericut, which will still not overcome the variables I mentioned above.

 

It is called Verify, not Guarantee.

[Jim at Gentex]

quote:

---

I am looking for stupid errors (on my part) that are going to cut the part in half, or render my fixture useless for the next part.

---

I'm with Zoober on this one.

I'm only using verify to make sure I didn't miss a tool retract or something that will cause a major problem.

 

Having said that, I've been having my own little hassle with verify that I haven't seen posted here yet.

 

X4MU1:

Write a toolpath,

Click on verify,

Load an stl file,

Verify looks good.

 

Write a second toolpath,

Try to run verify again on the same stl file...verify crashes.

 

Close Mastercam, then reopen,

Load the same stl file again,

Run verify on the 2nd toolpath,

All is well.

 

Write a third toolpath,

Try to run verify again,

crashes again...ad infinitum.

 

Anyone else had this issue?

[KMartin]

Thanks for the help Zoober

[cobra95kev]

Jim I have ran in to that too.

I have been making sure I hit save every single time now before I verify. Gotta love it.

[Zoober]

[malibu]

have too many problems with verify mill and lathe.

runing out of excuses with boss.

cnc do you have an oppening? just kidding but please, please fix it.

[Colin Gilchrist]

I know this won't help most of you, but there is software that can fix these "in-process" STL files. It is not cheap, but it is highly effective.

 

It is called Magics RP.

 

Zoober, I bet I could take your 800 Mb file and reduce it to about 50 Mb, with no loss in quality.

 

It is always overlapping or intersecting triangles that give you the fatal error. When you remove these from the STL file, Verify stops crashing.

[Zoober]

Colin, I had the demo.

It did everything you say it does and more. I didn't bother with the advanced stuff, just reducing the count, and repair. Worked with Sven a little to get going, but it was pretty easy.

It works like a charm. The company just doesn't want to spend the $$ at this time.

But I'm a-wishin......

[Colin Gilchrist]

I know!!! The cost is the #1 reason people don't get it. I really wish they would come out with Magics Lite or something like that. Just the healing tools, marking tools, filtering and reduction stuff. I don't ever touch the rapid prototyping functions. It sure is a pity because the software is worth it's weight.

 

If your company would buy it, I bet it would cut your verify time in half or better. It is literally that dramatic.

 

The other thing I love is using the tools to "bandsaw" off extra chunks of material off the STL. I get to remove the excess just like we actually do in the real world.

[Verndog]

Sometimes you just have to open up tolerances to get thru large parts and get on to something else. Mastercam verify hates faceting and bull nose 3-D roughing with small rads. A couple things to try without having Vericut. Filter toolpath to reduce faceting. Increase tool and STL tolerance in verify. This does not mean your STL will be off that far, just that more allowance is possible. Do not use transform STL to move part to new position, use tool plane in verify to move part op to op. In early operations use drop down speed / quality toggle toward speed before saving. (Run on quality to check, then drop down 2 notches toward speed to save and cut in the next operation)...this helps alot! Finally USE BACKPLOT!! Save GEO (make sure you are on endpoint backplot before saving) to new level and look for any discrepancies in toolpath GEO. Should be smooth and not be backing up on itself. Many gouges are the result of Mastercam losing which side to comp the tool on complex merging surfaces. Turn on a few surfaces (on their own layer) that could be problematic and gage toolpath GEO to those. In tight stitching often you can spot problem areas from weird or irratic moves (GEO)....and they DO happen.

 

This will eliminate 99% of issues without Vericut or other expensive "work around" softwares.

[Fred @ Slate Industries]

I just went down Jims road today with

Tech support, it's a Dead End.

[Chris Rizzo]

maybe it's time for cnc to think about licensing someone's decent verify product.

 

IMHO, that would have gone alot further than licensing fbm.

 

 

preaching to the choir

[Code_Breaker]

quote:

---

use tool plane in verify to move part op to op.

---

I seem to have missed this one ... where is "tool plane" in verify dialog box?

[Colin Gilchrist]

I think he is referring to "stock view" on the stock setup tab.

[Verndog]

quote:

---

I seem to have missed this one ... where is "tool plane" in verify dialog box?

---

Under the Files tab in machine properties use the Stock Setup then Stock View tab. You can pick a saved construction plane there to take the part from 1 orientation to another if the part moves from 1 machine to the next. Using this keeps from using Transform STL that can corrupt the STL and tend to waterfall surfaces that should be contoured.

 

1 easy way to pick and save tool planes. On original operation save 2 lines, a long X+ and a shorter Y+ from X0Y0. Save that GEO where you can find it later. After running operation xxx then part moves to new machine, pick the old X+ and Y+ lines and save the toolplane in a named view...say "OP1-STOCK". Then simply pick OP1-STOCK on next operation Stock View Tab and it will re-orient the part STL to your new coodinate sys.