Recommended Posts

I'd say yes, it's that bad.

This is what I get when I convert the file:

image.png.d90359736bd3fb4051482c2301028645.png

After deleting the sheet surfaces this remains:

image.png.8bebf33d38d1ed8e077cc25c43fe9493.png

  • Thanks 1

Share this post


Link to post
Share on other sites

Thank you, Richard, much better now. Any guitar guys want to share the best toolpath for the yellow highlighted area?. Is flowline best?. Thank you for the help. You guys rock.

 

Share this post


Link to post
Share on other sites

If you have the 5 Axis abilities Morph and from center out would be a solid choice. I would draw to long lines that are the range of the travel at the edges not the edges of the part. I would use them to drive the morph. Will get a cut along the same edge over and over again using that toolpath. Might look at breaking into surfaces splitting down the center and then using a center line to drive that toolpath. Then you can star from the top and work you way down both sides.

Share this post


Link to post
Share on other sites
38 minutes ago, C^Millman said:

If you have the 5 Axis abilities Morph and from center out would be a solid choice. I would draw to long lines that are the range of the travel at the edges not the edges of the part. I would use them to drive the morph. Will get a cut along the same edge over and over again using that toolpath. Might look at breaking into surfaces splitting down the center and then using a center line to drive that toolpath. Then you can star from the top and work you way down both sides.

Just a very nice 3 axis router. I like the start at the top idea. Scallop works for top down too.

Share this post


Link to post
Share on other sites
16 minutes ago, poolrod2 said:

Just a very nice 3 axis router. I like the start at the top idea. Scallop works for top down too.

Nope I meant do you have the 5 Axis add on for Mastercam. You can do 3 Axis milling with a lot of the toolpaths, but have to have a 5 Axis seat to gain access to them.

Share this post


Link to post
Share on other sites

Surface Finish Blend requires you to make chains. I love it, but I've been having great success lately with Surface Finish Hybrid. The motion is a mix between Waterline, and 3D Scallop. Play with the Limiting Angle. Sometimes 60 deg. is best, sometimes 45 or 30. But somewhere there is a perfect angle value that will make a pretty flawless finish path.

  • Like 1

Share this post


Link to post
Share on other sites
4 hours ago, C^Millman said:

Nope I meant do you have the 5 Axis add on for Mastercam. You can do 3 Axis milling with a lot of the toolpaths, but have to have a 5 Axis seat to gain access to them.

Got it, thank you.

Share this post


Link to post
Share on other sites
3 hours ago, Colin Gilchrist said:

Surface Finish Blend requires you to make chains. I love it, but I've been having great success lately with Surface Finish Hybrid. The motion is a mix between Waterline, and 3D Scallop. Play with the Limiting Angle. Sometimes 60 deg. is best, sometimes 45 or 30. But somewhere there is a perfect angle value that will make a pretty flawless finish path.

I will try it, thank you.

Share this post


Link to post
Share on other sites

My surfaces are pretty choppy, would one smooth surface be better?. Not that I'm good enough to achieve that ha ha. You guys rock. Thank you for all the help.

Share this post


Link to post
Share on other sites

Here is an out of the box version . .... Pencil . The old school version would not succumb to my wooing , but  the High Speed did.  Pencil looks for  two surface tangent areas ,  which usually  follow a very favorable direction of cut . Now  as the out of the box gemetry has internal corners  only in the end parts of the  neck geo , you would end up with  a smooth   

toolpath  , but  one which runs diagonally to the long direction of the neck . So how do we nudge pencil to cut along the neck ? 

1. we do a small incision on the top of the  neck . That will give you an along  bitangency .5a6c2c2dd9824_theslit.thumb.png.d10b884c9d1bf3b90bfb36d4fe121ea7.png5a6c2c636a47a_pencil1.thumb.png.e77b49ca34a6e626cf7d13fb6efe0d13.png

However if you feel that this incision  of  0.6 mm will be picked up by the fingers of a neurotic rock and roller ,  you  can  create a very  narrow patch of surface and 

raise it above the top of the neck .  mine  was 0.1 mm (0.004 inch ) and  I raised it above the neck of the surface  also 0.1 mm . And I got the same end result  as seen below 5a6c2eb4b50c1_theslither.thumb.png.3d48e76f7e2d6069b6567867cc57a6ca.png5a6c2f67bc1b3_thebestsolution.thumb.png.51ce3bf847e70269319194e344a159cf.png

 

  • Like 1

Share this post


Link to post
Share on other sites
On 1/26/2018 at 12:40 PM, Colin Gilchrist said:

Surface Finish Blend requires you to make chains. I love it, but I've been having great success lately with Surface Finish Hybrid. The motion is a mix between Waterline, and 3D Scallop. Play with the Limiting Angle. Sometimes 60 deg. is best, sometimes 45 or 30. But somewhere there is a perfect angle value that will make a pretty flawless finish path.

I only found Hybrid in Surface High Speed Toolpath, is that the one?. It looks like a lot of work to set up also.

  • Like 1

Share this post


Link to post
Share on other sites
21 hours ago, poolrod2 said:

My surfaces are pretty choppy, would one smooth surface be better

One of the great things about Blend is that it deals with "not perfectly" trimmed surfaces better than most toolpaths.

With Flowline, for instance, if I can't easily make a single surface from derived geometry from the part I usually move on to something else, maybe I will stick with it if I have to do only 2 or 3 surfaces separately......but generally I am using it to do corner rads. so I can make a single swept surface easily.

On the whole fewer surfaces the better, but the world has engineers in it so it's not always possible.

  • Like 1

Share this post


Link to post
Share on other sites

Making Flowline work in  cases like this is quite dicey .  Moldplus has an option to redefine your UV directions..

But back to the main story . I timed this . The setup was four minutes , importing the stp file  , drawing the  2d boundary , create curve from edege and draft surf creation + moving it  alon z 0.001 .  

As I am  metric I don't have the "feeling" of what is appropriate  in inch , so  finding the right value for overthickness which is the trigger value for the whole thing took two three shots at it. the metric version looked better .

 

 RR-COMPLETED 2017 RAINIER pullo inch.mcam

Share this post


Link to post
Share on other sites
17 hours ago, pullo said:

Making Flowline work in  cases like this is quite dicey .  Moldplus has an option to redefine your UV directions..

But back to the main story . I timed this . The setup was four minutes , importing the stp file  , drawing the  2d boundary , create curve from edege and draft surf creation + moving it  alon z 0.001 .  

As I am  metric I don't have the "feeling" of what is appropriate  in inch , so  finding the right value for overthickness which is the trigger value for the whole thing took two three shots at it. the metric version looked better .

 

 RR-COMPLETED 2017 RAINIER pullo inch.mcam

Thank you. I will try it.

Share this post


Link to post
Share on other sites

Ok guys, I'm trying the Surface High Speed Hybrid, it looks a little rough and takes around 3 hours to run this side. Any help would be great.20180210_092331.thumb.jpg.eba0b979b3913b54f8d3e258566e7b46.jpg

20180210_092230.jpg

Share this post


Link to post
Share on other sites

I would never use a bull endmill to finish a surface like that. A ball endmill is the better choice with a bull I would expect to get a far worse surface finish. No one is going to program your part for you. Share your Mastercam file through and external link, but no Mastercam file means you want someone to do your work for you.

Share this post


Link to post
Share on other sites
8 minutes ago, C^Millman said:

I would never use a bull endmill to finish a surface like that. A ball endmill is the better choice with a bull I would expect to get a far worse surface finish. No one is going to program your part for you. Share your Mastercam file through and external link, but no Mastercam file means you want someone to do your work for you.

I tried a 3/8 ball and it was really bad.

Share this post


Link to post
Share on other sites
58 minutes ago, poolrod2 said:

I tried a 3/8 ball and it was really bad.

What were you using for feeds speeds and stepover?

.5 - .75mm stepover, 20krpm, 10000mm/min, should yield decent results if the part isn't flapping in the breeze.  Should be easily sandable with 150 or 220 paper.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • 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