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:

Morph Between 2 Curves Example


crazy^millman
 Share

Recommended Posts

Okay I always talk about Morph between 2 Curves. I use it so much I just about forget how powerful a toolpath it is. I ran into an tricky one. Cutting Ti part with a port sticking on the side of the turned part. I cannot share the part, but I can share the solution to the problem.

 

#1 Create the toolpath like I want using .1 spacing for the toolpath. (You have to look at the file 10 steps here)

 

#2 Backplot the toolpath and turn on vectors in backplot.

 

#3 Save the Back plotted toolpath to a level.

 

#4 Figure out how much of the vectors need to be removed to not crash the tool into the body and delete them.

 

#5 Use the same toolpath an change to use Line in the tool axis control and closest to surface. (6 more steps here)

 

There are a lot more nuggets of information in this file that just these 5 things. File is on my Mastercam Shared Dropbox folder so it will stay active as long as I can pay the Dropbox bill.

 

https://www.dropbox.com/s/nahfak3wb3bp2l4/5TH%20AXIS%20MORPH%20CHEAT.mcam?dl=0

 

You have specific questions about this file then place ask and I will do my best a time permits to answer those questions.

  • Like 6
Link to comment
Share on other sites

Any reason you can't use the collision strategies to have the toolpath angle away when the holder nears that surface. I love what you've done here but i'm wondering why we can't get it to work using the tilt away collision strategy?

 

It doesn't work it kept freaking out the toolpath using them. That was my 1st thing to try. That was not giving me the desired results so I old schooled it.

Link to comment
Share on other sites

Installment 2. The back side of the area radius work.

 

You will see a single surface here. I tried using the original surfaces and with the solid and the surfaces it freaked out. I will not go into details how I created the net surface, but will if anyone wants that explained.

 

Here I only used 6 control lines for the toolpath to give you a different idea how to go about it.

 

https://www.dropbox.com/s/jebffifysdlebet/5TH%20AXIS%20MORPH%20CHEAT%202.mcam?dl=0

Link to comment
Share on other sites

It doesn't work it kept freaking out the toolpath using them. That was my 1st thing to try. That was not giving me the desired results so I old schooled it.

Yes i tried and got to that point also. i got close with a tilt away with a limit on the tilt but for some reason the blend spline is all wonked up between cuts.....Other than that motion looks good. That what i love about mastercam there is always a way to get something done.

Link to comment
Share on other sites

Yes i tried and got to that point also. i got close with a tilt away with a limit on the tilt but for some reason the blend spline is all wonked up between cuts.....Other than that motion looks good. That what i love about mastercam there is always a way to get something done.

 

When I did the big cone the collision with tilt worked perfectly using the geometry I was machining in the 1st example.

 

Scratch that spoke too soon. Need to create lines for that area also.

Link to comment
Share on other sites

There is one other way to handle the wonky tool stuff. Backplot the toolpath and use Curve 5 axis with the tilt lines.

 

The other dreadful and painful way is toolpath editor. Yes point by point and delete all the offending wonky points. 4100kb NCI file is 36793 points to sort through. Oh joy. :help: :help: :help:

Link to comment
Share on other sites

There is one other way to handle the wonky tool stuff. Backplot the toolpath and use Curve 5 axis with the tilt lines.

 

The other dreadful and painful way is toolpath editor. Yes point by point and delete all the offending wonky points. 4100kb NCI file is 36793 points to sort through. Oh joy. :help: :help: :help:

 

Update on this. 2017 handles my issue much better. Not exactly what I wanted, but no crazy rapids or anything so 2 thumbs up for fixing this issue.

  • Like 1
Link to comment
Share on other sites

Update on this. 2017 handles my issue much better. Not exactly what I wanted, but no crazy rapids or anything so 2 thumbs up for fixing this issue.

 

Okay I am very determined to get a toolpath exactly what I want out of Mastercam. I have well over 15 hours on this one section and not good enough to just  give someone a 3+2 toolpaths 4 different times around a part and say I hope your .01 profile tolerance on this Ti part comes out like you wanted. Now the toolpath has limited movements and be as smooth of a fluid motion as it can be. I still cant get one section to give me exactly what I want, but I could get what I wanted using a very different way of going about it.

 

In the toolpath there are limits for the tool axis control. I went to the XZ and limited the toolpath from 80 to 90 degree. For half of he part the toolpath is exactly what I wanted. Problem was it was going through the part and created just a mess. I was thinking man if I can get half to give me what I want I can live with that. t was just not there with surfaces and I was thinking how do I get here with a solid. I trim that thing 3 times and I got half of my solid and the section I want. I did that and got a nice 1/2 of the part along the center line and the front and back trimmed to just the section I need to cut. I re- picked those areas on my new solid and using limits of 80 to 90 degree got exactly the toolpath I wanted for half of the part. I then copied the solid and them swapped the trim to place and now have the other half of the solid. I coped the toolpath and picked those faces on the solid. I changed my limits to 260 and 270 and now the other half of the solid is cut exactly that way I want. Not to happy about the over lap in the center. I could backplot everything and save the geometry to a level. Get rid of the over lap and then use the drive to geometry with curve 5 Axis to make the toolpath one toolpath. I would use the saved vectors as my lines and get a toolpath exactly the way I want, but for now will submit to the customer and see if it works. If not then I will take that extra step to get no overlap half way, but maybe an hours more work if needed.

 

Once I can get to a place to make a file like the ones shared that don't voliate ITAR information I will try to post it up.

Link to comment
Share on other sites

Thanks Ron, I appreciate your sharing. I've been thinking about something along the lines of this myself, similar to the tips sticky but more of an example thread or how you would attack it thread.

 

 

So many different backgrounds and experiences it would be cool to see how others would attack stuff.

Link to comment
Share on other sites

Thanks Ron, I appreciate your sharing. I've been thinking about something along the lines of this myself, similar to the tips sticky but more of an example thread or how you would attack it thread.

 

 

So many different backgrounds and experiences it would be cool to see how others would attack stuff.

 

What I have done for over 13 years is share information. I want to help the industry using whatever tools I have. Mastercam has allowed me to do things I may not have otherwise been able to do in my life. I am thankful Jim Gamble the Mastercam dealer in Florida came in the shop I was running back in 2000. I owe a lot of credit to the Lord to giving me the gifts he has given me.

 

Side effect of all this effort is I can stick the tool into the holder a .250 deeper. I might can even get it down to 1/2 stick out in a shrink fit holder. On Ti that makes all the difference in the world on a Mill Turn Machine.

 

I did stick it down to .5 out of the holder.

Edited by 5th Axis Consulting Group
  • Like 1
Link to comment
Share on other sites
Installment 2. The back side of the area radius work.

 

You will see a single surface here. I tried using the original surfaces and with the solid and the surfaces it freaked out. I will not go into details how I created the net surface, but will if anyone wants that explained.

 

Here I only used 6 control lines for the toolpath to give you a different idea how to go about it.

 

https://www.dropbox.com/s/jebffifysdlebet/5TH%20AXIS%20MORPH%20CHEAT%202.mcam?dl=0

 

 

Sent from my SM-S902L using Tapatalk

 

 

Link to comment
Share on other sites

Ron,

Thank for that tip I could used that a few weeks ago. great job of thinking outside the box. I used to do a lot of little tricks back in the day in the software and once in while I forget that in most cases we are not limited to just what it wants to do.
This thought would helped on a inconel part I just did on a 5th.

Link to comment
Share on other sites

Wait just a goll darn minute. Morph between 2 curves? MC has a toolpath called morph between 2 curves?

 

Does it look shockingly similar to this?

 

MBTC_zpsvpftw9p3.jpg

 

Lets just say Moduleworks has a toolpath named Morph between 2 curves.  :sofa:

  • Like 3
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...