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:

Question on Backplot Times


ujmujm
 Share

Recommended Posts

I did 30 tool paths using the Dynamic Mill toolpath to rough out a part and when I backplot them to get a time I get  35 minutes but the operator tells me its taking 2 hours and he says he  didn't change a thing, I know the backplot times won't match machine times but I've never seen them that inaccurate, any ideas?

 

Link to comment
Share on other sites
27 minutes ago, ujmujm said:

I did 30 tool paths using the Dynamic Mill toolpath to rough out a part and when I backplot them to get a time I get  35 minutes but the operator tells me its taking 2 hours and he says he  didn't change a thing, I know the backplot times won't match machine times but I've never seen them that inaccurate, any ideas?

 

Depends on the machine, maybe your acceleration is not very fast, you could try increasing the minimum arc size and/or switching to zig zag mode if it is not zig zag mode you can increase your backfeedrate

Using microlifts?

Link to comment
Share on other sites
2 minutes ago, ujmujm said:

After confirming the run time turns out its 54 minutes not 2 hours but that is still way of the backplot time of 35 minutes, I've never seen that much discrepancy, must the age of the machine.

Rapid at 100%?

Link to comment
Share on other sites

Mastercam has no ability to calculate the accel/decel of your machine. The tighter the tolerance, the more any high speed machine is gong to slow down in the corners. The only way to make the times be closer would be to loosen the tolerance control values or eliminate cycle 32, however, I have no doubt you would end up with poor quality parts.

Carmen

 

Link to comment
Share on other sites

These are just roughing toolpaths so quality is not important as speed, but for these machines I have to go to Arc Filter/Tolerance and loosen the tolerance or the code won't fit in the control, you do make a good point that accel/decal is not up to the challenge. old machine new technology toolpaths.

Link to comment
Share on other sites
Just now, ujmujm said:

These are just roughing toolpaths so quality is not important as speed, but for these machines I have to go to Arc Filter/Tolerance and loosen the tolerance or the code won't fit in the control, you do make a good point that accel/decal is not up to the challenge. old machine new technology toolpaths.

I have done it on old machines and filtered it and turned the tolerance up to 10-20% of the stock I am leaving. If am leaving .1 then I will kick the total tolerance up to .01 or .02. I also turn on the use arc settings. As much as I would like to have a 25-30 year only machine run what a new machine does just not going to happen. Did a part for one customer on their HST Gantry at 24k rpms and 1200 ipm roughing a part. They sub out to a vendor who only has 5k rpms and we were lucky getting 150-200 ipm. Unless you go in and dial everything in and see what is the reality of the machine and match that in your toolpath your time will be off. If it is slowing down in the corners then you have a choice you can make that part of the toolpath to match the machine so your run time in Mastercam will match. Problem is going to be you get 1000 extra liens of code with all the changing feed rates because you must have Mastercam match the machine. It is a give and take on old equipment. 

Link to comment
Share on other sites

I have seen Dynamic Optirough be like this even on newer machines with High Speed Look ahead.  20 minutes longer on a 20 year old machine, to me, isn't that bad!  What everyone has said here is correct based on what work I have done as well.  I only have one machine where all of my programs match what Mastercam puts out, and it is only 1 year old.

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...