TOM S

Mirroring toolpaths without mirroring direction of cut

Recommended Posts

I need to machine 2 parts which are mirror images of each other.  I have programmed the first one.  I will mirror the geometry to create the second one.  Is there a faster / easier way of changing the toolpath?  I usually "reverse" and "change side" each operation individually, alternatively I have exported and imported the toolpath group and rechained the geometry.  

Both methods can be time consuming.  It seems to me there must be a better way when a complete part is mirrored to automatically reverse the chaining.  Am I missing something?

Share this post


Link to post
Share on other sites

Toolpath Tranform, Type Mirror , Method :Coordinate , Source: Geometry

Gracjan

  • Thanks 1

Share this post


Link to post
Share on other sites

It's the Source :Geometry that is the deal breaker here....

Gracjan

  • Thanks 1

Share this post


Link to post
Share on other sites
Guest
23 hours ago, TOM S said:

I need to machine 2 parts which are mirror images of each other.  I have programmed the first one.  I will mirror the geometry to create the second one.  Is there a faster / easier way of changing the toolpath?  I usually "reverse" and "change side" each operation individually, alternatively I have exported and imported the toolpath group and rechained the geometry.  

Both methods can be time consuming.  It seems to me there must be a better way when a complete part is mirrored to automatically reverse the chaining.  Am I missing something?

What version of Mastercam do you use?

A chook or nethook could automate your chain reversal across multiple operations.

I think this is a good point the software should do it, I've been in this situation lots of times.

Share this post


Link to post
Share on other sites
1 hour ago, Thee Byte™ said:

What version of Mastercam do you use?

 

I am running Mastercam Router 2021 with Curve 5 axis

I don't know much about chooks or nethooks, but will start looking into them.

The Toolpath Transform the pullo (Gracjan) suggested worked perfectly.

It seems to me though that perhaps Mastercam should automatically do this, or prompt you when mirroring geometry associated to an existing toolpath.  But perhaps I am a rare exception...

 

Share this post


Link to post
Share on other sites
51 minutes ago, TOM S said:

 

It seems to me though that perhaps Mastercam should automatically do this, or prompt you when mirroring geometry associated to an existing toolpath.  But perhaps I am a rare exception...

 

You are not the exception

  • Like 2

Share this post


Link to post
Share on other sites

This might not work as well on a 5-Axis Path, but I've had some decent success with making "As Shown" and "Opposite-Hand" parts, by creating a series of "Transform > Mirror (Geometry-Type)" Paths.

The real trick is to not try and grab "all operations" in one-shot.

I typically will do "groups of operations", where I know I want to perform the same "modifications" on everything. For example, "swapping lead in/out", "Reversing", Maintain Start Point/Entity".

 

Transform Mirror - Reverse Order.PNG

On 4/8/2021 at 8:25 AM, TOM S said:

I need to machine 2 parts which are mirror images of each other.  I have programmed the first one.  I will mirror the geometry to create the second one.  Is there a faster / easier way of changing the toolpath?  I usually "reverse" and "change side" each operation individually, alternatively I have exported and imported the toolpath group and rechained the geometry.  

Both methods can be time consuming.  It seems to me there must be a better way when a complete part is mirrored to automatically reverse the chaining.  Am I missing something?

The reality is: it is never as easy or as straightforward as you would expect it to be.

Honestly, I will typically use Mirror to create "new Operations and Geometry", because it is often easier to just have the new geometry/operations, so you can fix the Ops, without having to rely on a "source operation", and maintain that associativity. It just gets to be "too much", when you've got a part with dozens or sometimes hundreds of Operations.

It is the same reason I still use "Surfaces" for much of my toolpath operations. I want to be able to keep groups of Operations "semi-independent" from each other.

  • Like 2

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