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:

Ball nose not hitting edge of part?


Recommended Posts

So I have a program it is basically a pyramid, but one side is flat. The program works great ball nose and all but the corners on both sides that connect to the flat side don't get all the way done (where the yellow is in the picture). The ball nose doesn't go over far enough to actually finish it off. Im using waterline to do the ball nose. Is there something in the program that can tell it to go out a little more without me having to draw the part slightly bigger?.

Screenshot (11).png

Link to comment
Share on other sites

I tend to avoid waterline due to the tricky parameters and sometimes unexpected leftover material and containment boundary issues, you might want to try surface finish contour instead if you want a fancy operation ,or good ol fashioned one surface flowline my personal favorite.

Link to comment
Share on other sites

No surface finish contour is all about constant z stepdown and continuous chains, while surface finish flowline will "hug" the surface exactly machining only the selected area provided there are no checked surfaces or lead in out specified.Are you using any check surfaces btw because that can affect your toolpath in the way you described.

Link to comment
Share on other sites
19 hours ago, Nightsky84 said:

Is there something in the program that can tell it to go out a little more without me having to draw the part slightly bigger?.

Couple of things you can do. 

You could create a surface from the solid faces in question and extend them past your current edge, select them as drive surfaces to force the toolpath over. Creating a fence surface would be another way to achieve this.

On the parameters page of  the toolpath there is a gap settings button (legacy surfacing toolpaths) which allow you to extend the toolpath by length and angle.

Flowline would be the easiest as it doesn't require a containment boundary, but I am sure I could get an equally effective toolpath with Waterline or SFC.

Link to comment
Share on other sites

There's more than one way to skin this cat....using Waterline, I would approach it this way.

I pulled surfaces off the solid, I untrimmed them, then extended the back edge .125...I created curves and trimmed back to shape accounting for the .125 additional length...

Then using a boundary, constrained the cut

K1hTAbP.jpg

https://www.dropbox.com/s/xxu76cl5u6gfe8p/OLD-BEAR MOLD_INSERT_3_.mcam?dl=0

 

JM2C HTH

  • Like 1
Link to comment
Share on other sites
On 8/14/2019 at 12:57 PM, Nightsky84 said:

Is there something in the program that can tell it to go out a little more without me having to draw the part slightly bigger?.

I was just rereading this....the reality is, if you are going to do surfacing, you ARE GOING TO HAVE to create supporting geometry many times...

Sure, you can throw a toolpath at something and there are times it can be acceptable but most times you need more control....

I'm from the school that you should plan on doing any and all geometry creation necessary to get the exact toolpath you want.

I suppose that might be part of the reason I have been successful over the years...I will do what  need to do to get what I want out of the software...I look for solutions, not shortcuts.

Just a little opining on my part....if you find any of helpful...

  • Like 2
Link to comment
Share on other sites

I couldn't open the Mcx because i am only on mastercam 2018, so i recreated something similar however I didn't have the same Issue looks like there is a setting that is giving you problems, in the linking parameters Under "fitting" is it set to "Machine entire pass" ?

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...