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:

X8 Simulation question


Maclaw
 Share

Recommended Posts

Hi Guys,

 

Does anyone know how to spot a collision in X8 Simulation? I mean not a holder to workpiece/fixture collision etc but when the tool engages an absurd amount of material (ex. a 1/2" cutter buried 1" in material taking a full-width cut). The question came to me when I had a complicated part being machined with OPTI AREA/ OPTI REST. The toolpath had a bug in it that I didn't spot on simulation before letting it run on the miller. My 1/2" endmill just snapped away when it attempted to mill thru a full-width cut being buried 1/2" in material with a feedrate of 200IPM. I'd be surprised if it lived thru such a heavy and couragous cut... ;-) And adverts on Youtube say that "the side step is never exceeded".... Now I have a problem because I don't believe it... I have another problem - I like the OPTI toolpaths too much to just let them go... Hence my question...

Sitting by the simulator and looking for such a collision could take ages and You still need luck to spot it without any automation (call it "too much cutting collision detection") :-)

 

Thanks for the help.

 

 

P.S. Does anyone know how to make the simulator remember the "5 axis" setting in the "FILE-OPTIONS" menu? It makes me wild changing that everytime I use it... Thanks again.

Link to comment
Share on other sites

I don't think there is a setting in MX's simulator.  Maybe there's something in Cimco or Verisurf that you can set to detect it.  I've had the same problem with 5-axis option not staying put.  Not sure why it does it but, for me, it doesn't do it all the time.  There are certain files that will switch to 3-axis and I was assuming this was do to something in the file being corrupt.  the simulator still worked fine, you just get that warning every time.

Link to comment
Share on other sites

I just noticed an x/y/z stop condition that you can set in the X8 simulator.  Maybe if you set your x value to a specific diameter, this will stop it.  I am going to try it and let you know what happens.

 

Update to post.  This did not work.  I never used this before but it did not stop on an x values that I set.

Link to comment
Share on other sites

The answer to all your questions is no unfortunately. Been there done that and gotten no help from cnc.

 

Was the overcut condition on a backfeed move? I just had a backfeed cut at 75% at 500IPM with a 2" facemill. It was because my step up was 6.25%. Apparently 6% doesn't trigger the bug. I had 100% faith in the Highspeed toolpaths. Now I don't.

Link to comment
Share on other sites

One thing you could do, is set the tool's "Cutting Length" under "edit tool" to the largest amount you want to allow... say .150"

 

Then, within the simulator, make sure you turn on "Shoulder" under Collision Checking.

 

That will check for any errors that go beyond the depth of cut you set.

 

As for the full width of cut... you should be able to see that in verify.

 

TBH, I've never had it take more than expected on a side cut.

  • Like 1
Link to comment
Share on other sites

Hi Guys,

 

Thanks for the tips. I guess some have to be addressed to Cnc Software for future releases / MU's...

 

Josh - the overcut wasn't on a backfeed - the toolpath went to do upsteps WITHOUT roughing out the stock first. When I changed the path boundries (see attached JPEGs) in either way - the problem dissapeared.

 

I still have no explanation for that - maybe someone from Cnc Software can help? Please.... It must be a bug issue. What is quite vital is that it happened to me in X7... So... The BIG QUESTION is -> was X8 more thoroughly tested and had all found bugs removed regarding the HST??? I think this is CRUCIAL for all machinists(no need to explain why) using MC. So... can someone from Tolland let us know about this...? I would be grateful... :-)

 

Anyway - I will try to put the "buggy" toolpath thru X8 - the exact file -  and will let you know about the results.

 

 

Reko - thanks for your suggestion - I'll give it a shot. I hope you will NEVER experience a "feed crash" with HST.

 

 

My feelings for HST in MC from now on also became a little bit mixed. I know OPTI (the "upstep" approach, stock awareness, etc.) is definetely HUGE! That's the road it should take - it's a BRILLIANT strategy! But - it must be (as close as possible to) PERFECT! This is a must - no questions asked. HST means running your machine tool at feeds that are corrsponding to RAPIDS in some older machines! That's nice, but also - serious. This is really where SECOND BEST won't cut it!

So - to the Creators - MAKE MC THE BEST! I believe in you!

......so does my maintenance bill....... :laughing:

 

Thanks again Guys!

 

 

 

post-45389-0-21629300-1414536272_thumb.jpgpost-45389-0-60967900-1414536269_thumb.jpg

 

 

 

Link to comment
Share on other sites

I put it through X8. Opened the old MCX7 file in X8 and made a regen on the "buggy" toolpath operation (it came in clean to X8 but I did a regen at it to let X8 toolpath algorithms overwrite the X7's). And guess what?

 

X8 made it right!!           :cheers:

 

That's definetely good news! This gives some proof (for me at least) X8 is more reliable and has less bugs in HST!. Good, because I was worried that X8 mainly changed with the graphics (which is also very useful and cool)..!

Well - my faith in opti and HST grew slightly, looking at X8 from this point of view. I hope this doesn't change. We'll see what the future brings....  :guitar:  

Link to comment
Share on other sites

I have been using Opti tool paths in X8 a lot and haven't had this problem, if anything I've had problems with Opti tool paths not going into areas that I want them to.  But, like you said, this needs to be perfect because the feed rates that run with this tool path are not forgiving.  I'm glad X8 fixed it. 

Link to comment
Share on other sites

Hi Guys,

 

 

 

 

P.S. Does anyone know how to make the simulator remember the "5 axis" setting in the "FILE-OPTIONS" menu? It makes me wild changing that everytime I use it... Thanks again.

 

I found this on Mastercam.com in their knowledge base.  Not sure if it would be the same for X8 but it might be worth a shot.  This shows how to force X7 to always choose 5-axis.

post-52370-0-67305300-1414615190_thumb.jpg

Link to comment
Share on other sites

One thing you could do, is set the tool's "Cutting Length" under "edit tool" to the largest amount you want to allow... say .150"

 

Then, within the simulator, make sure you turn on "Shoulder" under Collision Checking.

 

That will check for any errors that go beyond the depth of cut you set.

 

 

 

Reko - it's a good idea - I've just tried it out on the "buggy" operation I was talking about. It sure well stopped in the place where it wanted to engage too much DOC. Thanks again for the tip.

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

  • 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.

Follow us

×
×
  • Create New...