X6 Optirough Major failure!

[Thee Rickster ™]

IMHO, +1's and -1's are for sissy's!

[neurosis]

Bob,

 

Ive sent this file to my reseller already (he was a little irritated with me for posting the video on youtube ) and am waiting for a response from Q.C. before sending it to them.

 

My intention was not to post the video on youtube to make a mockery, it was an 80 meg video and i wanted to be able to send it several places easily including this forum.

 

I would like to know, assuming I did not cause the problem myself (i cant imagine that is possible when you see what is happening) if they plan on giving a work around for the problem or releasing some kind of patch in a timely manner. If this is something that we have to wait 6, 8, 10, months to have fixed then there will be some serious thinking going on in our front office along those same lines.

 

This is not a small issue. This could possibly cause a machine crash. Right now the only work around that I see is to change the retract to full vertical or change the back feed distance to a retarded number neither of which is an option. It would add too much time to some of our parts and not be worth the effort.

[Joe788]

Dont get me started on that again.. haha.

 

But yes... with these flaws in X6 ive already been told by the owner and foreman that we are not to use X6 for production. This is B.S. because now we have to wait for who knows how long to get a bug fix and as we already know, Mastercam/CNC does not release patches. I am sure that when our maintenance comes up for renewal I am going to be in the position of having to argue the case to continue it again with the same comments that I hear every single time. "Why am I paying to beta test their software?" "Where is our return when the software does not work properly" and until then, "When are they going to fix these issues so we can use what we have already paid for!" They make me feel as if these issues are some how my fault some times. Although in their eyes, it is MY fault that we are still using this software because I am the one that has continued to convince them to keep it.

 

And it definitely is a bummer about volumill.

 

The biggest bummer is that your stock model is crashing. I've become a stock model junky over the last few months. Haven't had a crash with it yet. I also always use full vertical retract on Optirough so I haven't seen the crashes on that either.

[?Mark]

Who would give a -1 for that?

 

John, I gave one of my +1's for the day to you because -1 - ing that is just... just.... nevermind.

 

i did too...

[Newbeeee™]

Just looked at the vid on youtube and see that Jonny boy has made a couple of comments

[neurosis]

I'll delete his comments.. I dont want his bullxxxx linked to anything that we do or say here at our shop.

[neurosis]

I think that I may have found a temporary solution to the problem.

 

When I am using these tool paths to rough steel, especially on our older machines, I always change the vertical arc entries to 0. They produce too much code and when you are feeding at 20 ipm, they are pretty much useless.

 

Well, I changed my arc entries to .01 and regen the tool path and wallah! The cutter cleared the material on every pass.

 

I sent this info in to QC but not sure that they will be getting back to me. I would like to get some feed back from them on this.

[Zoober]

I got a bug report cnc00053697 back in 09 covering the vertical arc entry in rest roughing. Sounds and looks the same as what I went thru

[Newbeeee™]

I just added an enhancement request in the enhancement forum for verify regarding this. I must admit it is something that has always 'worried' me as the high back feed rates if they clip metal, would obviously cause tool breakage.

As verify doesn't pick this up and it's rediculous to try to go through the code as there's so much to see with these toolpaths (not knocking them as they are exceptional), a verify change I think is in order?

Please have a look and comment.

cheers

[neurosis]

Ok, I got a response from my VAR yesterday and what he told me I do not think was correct so I want to ask the guru's here for their opinions and ideas.

 

 

His response to me was, that in your Linking Parameters, you have to set your Linear entry/exit(incremental) to a greater distance from the depth of your cut, what ever that might be, to the clear distance of the top of your part.

 

There are several reasons that I dont think that he is correct but I would like to get a response from someone that knows for sure. Arent the "Leads" in the high speed tool paths nothing more than the lead in and lead out control and the "Part clearance" what controls the distance that the tool clears the material?

 

I have NEVER had to set this or or any of the Leads values to any such numbers in the past. I could leave every number in the "leads" @ 0.0 and have never had a tool crash through material this way.

[Newbeeee™]

Arent the "Leads" in the high speed tool paths nothing more than the lead in and lead out control and the "Part clearance" what controls the distance that the tool clears the material?

 

That's my take as well. We have defaults set and never change them and have never had a problem...knock on wood

[neurosis]

What do you use for your "Leads" values?

[Tyler Robertson]

that sounds more like a workaround - a lead in should be able to be whatever distance you want it to be, same with clearance

[neurosis]

that sounds more like a workaround - a lead in should be able to be whatever distance you want it to be, same with clearance

 

 

That was what my response to him was. That is sounds more like a work around than a solution. I told him that I could also fix the problem by changing my clearance to "Full Vertical Retract" and accomplish the same thing but that would also only be a work around and just as his work around, it would create a very inefficient tool path. Who wants to run this path if they have to retract above the top of the part ever single pass? We use this path in pockets that are some times 6" deep with various islands and other features. There are literally 1000's of passes in the pockets and if I had to retract above the top of the part for every single pass in order to not high speed feed through material I would NEVER use these paths.

 

He also never replied back to me when I asked him that if this were the true solution to the problem, why did this crash not happen in X5? This file was pulled in from X5 and not a single change was made to the parameters. I just regenerated the path and it crashed through the wall.

 

Not only that, but if you notice, the first pass actually clears the part as intended. It is the NEXT pass that high feeds through the material.

 

When I asked him these questions he stopped responding to me.

 

I am little pissed because our VAR posted a video after I posted mine, stating that the Vertical Lead is the solution but he is misleading people which I feel is wrong even though it is more than likely unintentional.

[Thee Rickster ™]

So Comment on his video then.....

 

and direct him to this thread....

[neurosis]

I tried to comment on their video but he didnt allow it.

[Newbeeee™]

What do you use for your "Leads" values?

 

Entry / Exit 2.0mm (.080")

Vertical arc entry 1.0mm (.040")

Vertical arc exit 1.0mm (.040")

 

Fitting = Minimise Trimming

Max Trimming distance 1.1mm (.044")

 

Minimum vertical retract set at default

 

And that's it really.

It would be REALLY nice if there was a quick and dirty guide available for these paths. That said, these have been our defaults since we started using the paths and haven't had a prob.

[Newbeeee™]

So Comment on his video then.....

 

and direct him to this thread....

I expect Jonny Bonkers has already...

[neurosis]

I've always left the vertical arc entries at 0 because they generate too much code. I set the vertical to .1 so that it slows down prior to feeding in to the material. I always have a horizontal arc entry of .1 or more depending on my feed rate.

 

The explanation that I got from CNC said that I was using the settings properly. Part clearance should take precedence were the exact words used. So I should be able to leave all of the Lead values to 0 and if I have a .5 part clearance set, then it should always clear by .5.

 

Its a little frustrating to be mislead in to thinking that you are using a function improperly. Its taken that much more of my time to deal with the situation only to find out that we were indeed using the function as intended.

[Jim Evans from CNC Software]

Sorry for being late to the game folks, but I was out of town on vacation and just getting back into things here. We have the developer looking into the issue and it does have to do with the vertical arc entry being set to zero. Not sure why yet but we are looking at it and figuring how ho to provide a fix. That fix could be a patch or a re-release of X6. More to come as I get details.

Jim

[neurosis]

Thanks Jim!

 

I figured out later yesterday that if I added a value of even .01 to the arc entry the tool would clear.

 

That is the work around that I have been using and so far things have been working flawlessly.

 

Patiently awaiting the patch or re-release.

[Thee Rickster ™]

Jim, can you guys check all the little issues/bugs that have arose, including some that are still

present in X5? It would be nice if they were addressed too.

 

Thanks

[neurosis]

Jim, can you guys check all the little issues/bugs that have arose, including some that are still

present in X5? It would be nice if they were addressed too.

 

Thanks

 

 

+1

 

Including the issue that I posted Here

 

The cutters are honestly feeding IN to the material at the back feed rate. It is an insert shocker to say the least.

[CamMan1]

Sorry for being late to the game folks, but I was out of town on vacation and just getting back into things here. We have the developer looking into the issue and it does have to do with the vertical arc entry being set to zero. Not sure why yet but we are looking at it and figuring how ho to provide a fix. That fix could be a patch or a re-release of X6. More to come as I get details.

Jim

 

 

We have the "developer" looking into the issue and it does have to do with the vertical arc entry being set to zero. I thought CNC Software Claimed that they developed these toolpath strategies?

[Colin Gilchrist]

We have the "developer" looking into the issue and it does have to do with the vertical arc entry being set to zero. I thought CNC Software Claimed that they developed these toolpath strategies?

 

This developer is a direct employee of CNC Software. He works here in the building. Is there a purpose to your comment?