Sign in to follow this  
cncasylum

Silhouette Boundary

Recommended Posts

Hello everyone hope all is well.

I am having a hard time getting  what i am looking for.  When grab my solid  for a silh. boun. I'm not getting an exact replica of my boundary. I'm getting broken arcs with different rads by a couple of thou. Its not that big of a deal in this application but i mill sprockets also where the rad on the teeth are very critical. 

Shutter.ZIP

Share this post


Link to post
Share on other sites

I've never found Silhouette Boundary to be accurate enough for finish geometry. I only use it for rough and rough boundaries

 

Sounds like in your use, Create >> Curve > Slice would be a better option

  • Thanks 1
  • Like 3

Share this post


Link to post
Share on other sites
6 minutes ago, cncasylum said:

Hello everyone hope all is well.

I am having a hard time getting  what i am looking for.  When grab my solid  for a silh. boun. I'm not getting an exact replica of my boundary. I'm getting broken arcs with different rads by a couple of thou. Its not that big of a deal in this application but i mill sprockets also where the rad on the teeth are very critical. 

Shutter.ZIP

Maybe tighten up the tolerance>?

  • Thanks 1

Share this post


Link to post
Share on other sites
14 minutes ago, cncasylum said:

Hello everyone hope all is well.

I am having a hard time getting  what i am looking for.  When grab my solid  for a silh. boun. I'm not getting an exact replica of my boundary. I'm getting broken arcs with different rads by a couple of thou. Its not that big of a deal in this application but i mill sprockets also where the rad on the teeth are very critical. 

Shutter.ZIP

For 100% accurate geometry, you are much better off using "Transform > Project", to take your actual part wireframe, and projecting it to a specific working depth.

The first thing I do when evaluating a "new model" that I'm working with, is increase my Analyze Precision, to at least 1 decimal place more accurate, than my machine's resolution. So for an Inch Part, with a machine that has 0.0001 Inch Resolution, I want my model geometry to be accurate to 0.00001 Inches. (10 millionths.)

If I'm working in Metric, and my resolution is 1 micron (0.001 mm), then I want my geometry to be accurate to 1/10th of that value. (0.0001 mm).

Every piece of geometry has an intrinsic tolerance associated with it.

Question: when is zero, not zero?

Answer: when your resolution isn't fine enough to "see" the geometric errors, due to rounding.

For example, if you've got a round part, and you move it to the System Origin, but your resolution isn't good enough to detect the error.

If you've got a part that is located at X 0.000032, and Y is 0.000041, is that properly located at the System Origin?

The answer is: "It really depends".

Based on 'standard rounding', yes, that part is located at X0. Y0.

But if you increase your Analyze Tolerance to 6 decimal places for Inch Mode, you'll clearly be able to detect that the part is off by 32 millionths in X and 41 millionths in Y.

In this example; the foundations of your part accuracy are not correct, and this may or may not lead to errors "downstream" in your programming.

In your example; you should verify that the part origin is located correctly, and that your Solid Model does not contain any errors. You can use the Model Prep Tools (Simplify Solid and Optimize), to fix errors in your model. Home Tab > Analyze > Check Solid can be a useful tool to also detect modeling errors.

 

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

Excellent. Thanks so much. A whole pile of usefull information. Definitely going to apply these fresh tactics. 

  • Like 1

Share this post


Link to post
Share on other sites

Good morning,

I'm am familiarizing myself with cleaning up my model. Home > analyze> check model definitely have problems but all lye within my engraving and u can see very clearly that lines don't meet up. Thinking I can remove the engraving to fix. Help said attempt to heal solid when opening option.  model pre> simplify solid> optimize show issues with engraving also. I can keep choosing this option and I get different numbers of errors. Do I need to go in and fix these issues and then run this feature again till I get zero or should I approach in a different fashion? Thanks for everyone's help this forum has proven to be a very valuable tool for my toolbox I wish I used more frequently years ago.

 

Screenshot (17).png

Screenshot (18).png

Share this post


Link to post
Share on other sites

Make sure you are modifying a copy of the original part on a new level. That way you always have the original solid within your file.

 

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites

What kind of engraving is it?

Is this just a Part Number or Serial Number which is getting engraved, or it is something like a company logo, were maintaining the look of the design/font-style is critical?

Most of the time, I will clean up my solids by removing a shallow pocket style of engraving (like you show), and simply create my own Wireframe (centerline of the characters) to drive the toolpath.

Mastercam recently added a new (simplified) font which is amazing for engraving. The characters are designed to not have branch points in the geometry, which makes it so easy to get clean Contour chains.

You don't have to repair all of those engraving issues with your model. > What I do is copy my solid onto a different level (Keep Original and make a new 'Manufacturing Model' on another level) , then i would create a 'surface from solid', on the face which contains the engravings.

Click this surface, and press ALT + E (hide), to display only that surface on your screen (temporarily).

Use the 'Remove Boundary' function on the Surfaces Ribbon.

Click the surface, and a Dynamic Arrow will appear. Slide it to the edge of one of the engraving pockets, and click. Mastercam will then prompt you: "do you want to remove all internal boundaries"? Click yes. Press ALT + E to restore your visible geometry on the screen.

Doing this should remove all of those character boundaries, while leaving any "exterior trim boundaries" intact.

Typically, I create an entire Surface model to drive my Toolpaths, and your example is the reason why. I do a similar process for filling any holes before roughing. Yes, you can create a 'cap surface' to fill a hole, but I prefer there to be no mathematical gap in those areas.

The cleaner your geometry is, the less the Toolpath algorithm has to do, to create clean G-Code.

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites

Love it thanks. These characters are just a part number basically showing where they want the graving. I'm going to look into the simplified font sounds like something id like to use.

Screenshot (19).png

Share this post


Link to post
Share on other sites
10 hours ago, cncasylum said:

Love it thanks. These characters are just a part number basically showing where they want the graving. I'm going to look into the simplified font sounds like something id like to use.

Screenshot (19).png

It's available in the Create Letters command. I think it is now the default font for that function.

We used to only have 'Stick Font' for a simple centerline geometry, when creating letters. You can still change the height and character spacing if needed. 

Share this post


Link to post
Share on other sites
On 1/13/2021 at 7:59 AM, cncasylum said:

Hello everyone hope all is well.

I am having a hard time getting  what i am looking for.  When grab my solid  for a silh. boun. I'm not getting an exact replica of my boundary. I'm getting broken arcs with different rads by a couple of thou. Its not that big of a deal in this application but i mill sprockets also where the rad on the teeth are very critical. 

Shutter.ZIP

Another way was to take all the wireframe on the same level as your solid and move it to a different level. Then copy the shape wireframe to a new level. Then project that to a plane where you wanted the shape to be and done. Here is your file back with levels explaining what I did as an example. Always use what you got when you got it helps to prevent possible errors when doing it other ways. Other ways mentioned are good ways, but I like using what I got to make what I needed. The arcs from Level 50 to 51 were 4 arcs for top and bottom. I used the join entities to make them both into one arch to each place on the part shape.

5th Axis Example with Wireframe and Project

  • Thanks 1

Share this post


Link to post
Share on other sites
On 1/14/2021 at 7:01 AM, cncasylum said:

...model pre> simplify solid> optimize show issues with engraving also. I can keep choosing this option and I get different numbers of errors. Do I need to go in and fix these issues and then run this feature again till I get zero or should I approach in a different fashion? Thanks for everyone's help this forum has proven to be a very valuable tool for my toolbox I wish I used more frequently years ago.

To expand upon the use and results of the Optimize command-

Optimize will never work itself down to zero, and by running it multiple times and seeing it bounce between different optimization numbers, you're basically trading the same two results sets back and forth in the background. If you use Optimize, running it once should net you basically all the benefits you will get. Good question!

  • Thanks 1

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
Sign in to follow this  

  • 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