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:

Machsim MCAM2020


JParis
 Share

Recommended Posts

Am I the only one that has seen Machsim become utterly useless in 2020?

It's not tied to my post but in versions since X9 I have been able to use it to check my part and tooling clearances, I have been setting a high Z retract to not have to worry about rotary interferences...

in 2020 it consistently mills through parts reporting no crashes...these are movements that are not going to happen in reality, 

9qtddHp.png

 

6SNZx8g.png

 

Like this, it's utterly useless to me

 

 

Link to comment
Share on other sites

Hi Jparis, i think your dogleg settings do that, to change them see below, there is an article on this in the Knolwegebase if you search Dogleg, this should fix that mach sim issue and this problem can also cause a verify issue too. 

  1. Go to the machine tab
  2. Choose machine definition
  3. Check out of the warning that appears, then the machine definition will open
  4. Click edit control definition
  5. Go to the linear page
  6. Choose Linear Interpolate at maximum feed rate for your rapid motion.
Link to comment
Share on other sites
2 minutes ago, JoshC said:

Hi Jparis, i think your dogleg settings do that, to change them see below, there is an article on this in the Knolwegebase if you search Dogleg, this should fix that mach sim issue and this problem can also cause a verify issue too. 

  1. Go to the machine tab
  2. Choose machine definition
  3. Check out of the warning that appears, then the machine definition will open
  4. Click edit control definition
  5. Go to the linear page
  6. Choose Linear Interpolate at maximum feed rate for your rapid motion.

Nope, not on this mess but thanks :cheers:

  • Like 1
Link to comment
Share on other sites
5 minutes ago, JParis said:

Nope, not on this mess but thanks :cheers:

oh bummer, i thought that would do it because it helped with a mach sim issue that i had today that was very similar to what you described, sorry i couldn't be more help, im sure cnc will have you an answer if you sent it there, have a good night.

Link to comment
Share on other sites

Our's is utterly useless as well, our documents folder is synced to the server and it makes launching the Machsim so slow it's not even worth the time.  It takes Mastercam at least 5 minutes close at the end of the day, everyone's workstation does it, not just mine.  The only thing I can come up with that would be the cause is the Sync Center.

Link to comment
Share on other sites

So going through all of the tool paths, I discovered something

There are 4 tools in the program, that if I include them in the simulation, other tools look as though they are ripping through the part.....if I leave those 4 tools out, everything looks fine..

It's strange that it isn't the tools in question that actually look bad but that it's causing other tools to look bad...

I sent the file in but at 602 operations, I needed to break it down further and resubmit it

Link to comment
Share on other sites
8 hours ago, JParis said:

So going through all of the tool paths, I discovered something

There are 4 tools in the program, that if I include them in the simulation, other tools look as though they are ripping through the part.....if I leave those 4 tools out, everything looks fine..

It's strange that it isn't the tools in question that actually look bad but that it's causing other tools to look bad...

I sent the file in but at 602 operations, I needed to break it down further and resubmit it

The problem is caused by "Dog leg rapid movement". As Josh had suggested. There is a bug in Mastercam X9, you have to double and triple check if the rapid motion has actually been updated. I bet the 4 tools that cause a problem are used to machine a number of operations at different planes before the tool change. Try to force a tool change in between operations.

Link to comment
Share on other sites
7 hours ago, Joe777 said:

The problem is caused by "Dog leg rapid movement". As Josh had suggested. There is a bug in Mastercam X9, you have to double and triple check if the rapid motion has actually been updated. I bet the 4 tools that cause a problem are used to machine a number of operations at different planes before the tool change. Try to force a tool change in between operations.

Well, I'll tell you what...

The 1st tool I caught that caused it a was tool 15......I'd certainly love someone to explain how it's a dogleg when adding tool 15 into the simulation caused tool 2 to look like it gouging...or why adding tool 28 causes tool 19 tool look like it's gouging?

My retracts are set to 12"

Believe me, it's NOT doglegs

 

Link to comment
Share on other sites

AKA...."computer voodoo"

Quote

 This is an issue with a small arc segment being flipped. I see arc filtering on in one of the ops that had the issue, and what's happening is that, in simulation, when we get to a small leadin/leadout arc on the end of one of the passes, the math being done to the arc move is incorrect and is flipping the solution, so instead of a 5 degree segment of arc, we get the inverse- 355 degree segment- and cut a big loop, which is not detected as a collision. The NCI, posted code, toolpath display, backplot display, etc, don't show this, because it's only flipping the arc at the moment we're driving the tool around for simulation. I haven't seen this issue in 2020 before.

 

Link to comment
Share on other sites

I've had this issue many times too. Couldn't figure out how to resolve it. But oddly in a large file(for this shop 200-300 operations), sometimes it would pick and choose where it wanted to start. It would sometimes start many tools down the list then go back and do other things. I've since resorted to just using the Verify instead since I don't have these issues there. 

Link to comment
Share on other sites
6 minutes ago, jwvt88 said:

I've had this issue many times too. Couldn't figure out how to resolve it. But oddly in a large file(for this shop 200-300 operations), sometimes it would pick and choose where it wanted to start. It would sometimes start many tools down the list then go back and do other things. I've since resorted to just using the Verify instead since I don't have these issues there. 

They(CNC Software) had to really dig to find it.....I should be getting a bug number shortly but between PM's, emails and phone calls we've got it sorted out....

  • Like 1
Link to comment
Share on other sites
1 minute ago, WestRiver said:

Let me know when it is all sorted out because I have it to.

It seems to be a calculation error on small arcs within Machsim, it's not the code, backploy, verify or nci....try turning off filtering and see if Machsim runs properly

There is also another issue tied to axis sub but that's not in play on my file

  • Thanks 1
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...