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:

surface toolpaths rolling sharp corners


Sigurd
 Share

Recommended Posts

I have fought this off and on since I started with 3D toolpaths. The photo show it. The cutter will either roll or gouge the top edge of a corner. I have gotten around this by creating a surface and extending it .005", but is there a setting that I'm missing? Backplot doesn't show this, Verify doesn't show this, but then there it is on the part. 

File is attached. Thanks for taking the time to look.

nozzle block B.mcam

gouge.jpg

Link to comment
Share on other sites

Hey Sigurd, I assume your problem here is unwanted cutting of the top surface of the part at the end of Toolpath 2 which is doing the cavity, and where we see the "Band" machined in your part picture that doesn't exist on the model.

What is likely happening here is that because you are using two different tools- 0.280 ball for Path 1 and 0.311 ball for Path 2- is that you have some slight error in the tool Height offset.

 

The way this is programmed is primed to show even the slightest height variance- Note here how Toolpath #2 takes a pass right at the sharp edge of the cavity. If those two tools are not perfect in their H offset down to the tenth of a thousandth, you'll get mismatch because you're essentially asking one path to remachine part of the other with a zero tolerance:

1504037710_Endofpath.jpg.3be8a49cdee3d8a16b37b1a249b654ed.jpg

 

Backplot and Verify/Simulation would never show this because of course in the computer world, all the tools are a perfect shape with perfect height offsets and no wear!

To avoid this situation, you could do something like Turn on Tool contact point in the Toolpath Control page, and then also go to Model Geometry and add the Top Face and Front Faces as Avoidance surfaces to clean up the motion that Tool Contact Point creates. I think you might be using Toolpath #2 as both a roughing and finishing path, so this may not be viable, but it's how I would avoid these "accidental" remachining circumstances. Another solution would be to finish both surfaces with the same tool, if possible. This will naturally avoid this tool offset problem you're encountering.

  • Like 2
Link to comment
Share on other sites

There are so many different ways to correct this issue.

Assuming your machine is in good working order and your tool geometry is good as well as your length offsets.

You could choose any/all of the following methods to correct it.

1 - choose the top surface as a check surface/avoidance surface

2- by using a boundary

3- by using Z depth limits

4- by using slope values. Only cut surfaces between 1 and 90 degrees of slope. ( assuming the top surface is flat/ zero degrees )

 

Carmen

  • Like 3
Link to comment
Share on other sites
On 4/18/2022 at 3:04 PM, Chally72 said:

Hey Sigurd, I assume your problem here is unwanted cutting of the top surface of the part at the end of Toolpath 2 which is doing the cavity, and where we see the "Band" machined in your part picture that doesn't exist on the model.

What is likely happening here is that because you are using two different tools- 0.280 ball for Path 1 and 0.311 ball for Path 2- is that you have some slight error in the tool Height offset.

 

The way this is programmed is primed to show even the slightest height variance- Note here how Toolpath #2 takes a pass right at the sharp edge of the cavity. If those two tools are not perfect in their H offset down to the tenth of a thousandth, you'll get mismatch because you're essentially asking one path to remachine part of the other with a zero tolerance:

1504037710_Endofpath.jpg.3be8a49cdee3d8a16b37b1a249b654ed.jpg

 

Backplot and Verify/Simulation would never show this because of course in the computer world, all the tools are a perfect shape with perfect height offsets and no wear!

To avoid this situation, you could do something like Turn on Tool contact point in the Toolpath Control page, and then also go to Model Geometry and add the Top Face and Front Faces as Avoidance surfaces to clean up the motion that Tool Contact Point creates. I think you might be using Toolpath #2 as both a roughing and finishing path, so this may not be viable, but it's how I would avoid these "accidental" remachining circumstances. Another solution would be to finish both surfaces with the same tool, if possible. This will naturally avoid this tool offset problem you're encountering.

I did intentionally use two different tools. A used one for roughing and a nice coated one for finishing. This was a hardened part. 

The top surface was finished in the grinder. I had no need to cut it.

I tried "contact point" and top and front avoidance surfaces like you suggested. Looks good. Next time I get some steel, I'll try it in the machine.

  • Like 2
Link to comment
Share on other sites
On 4/19/2022 at 3:15 PM, Redfire427 said:

There are so many different ways to correct this issue.

Assuming your machine is in good working order and your tool geometry is good as well as your length offsets.

You could choose any/all of the following methods to correct it.

1 - choose the top surface as a check surface/avoidance surface

2- by using a boundary

3- by using Z depth limits

4- by using slope values. Only cut surfaces between 1 and 90 degrees of slope. ( assuming the top surface is flat/ zero degrees )

 

Carmen

1. When I originally cut this last week, selecting the top surface as avoidance made the toolpath not run at all. It's fine now, but I'm not sure what changed.

2. I had been using a boundary.

3. I had been using max depth. Min depth was .005" above the part. I thought that would have the cutter end above the part. Is that my problem?

4. Ah. Steep/shallow. Got it.

 

Thanks for the help. I really appreciate it.

  • Like 1
Link to comment
Share on other sites
On 4/19/2022 at 3:15 PM, Redfire427 said:

There are so many different ways to correct this issue.

Assuming your machine is in good working order and your tool geometry is good as well as your length offsets.

You could choose any/all of the following methods to correct it.

1 - choose the top surface as a check surface/avoidance surface

2- by using a boundary

3- by using Z depth limits

4- by using slope values. Only cut surfaces between 1 and 90 degrees of slope. ( assuming the top surface is flat/ zero degrees )

 

Carmen

1. When I originally cut this last week, selecting the top surface as avoidance made the toolpath not run at all. It's fine now, but I'm not sure what changed.

2. I had been using a boundary.

3. I had been using max depth. Min depth was .005" above the part. I thought that would have the cutter end above the part. Is that my problem? What if I set it to -.0005" or something so that it never comes up to the top surface?

4. Ah. Steep/shallow. Got it.

 

Thanks for the help. I really appreciate it.

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...