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:

Deburring paths


medaq
 Share

Recommended Posts

Sorry, I have a lot of questions. :D

 

But since I am coming from pre x version, and moving to the new 2017-2018 version. 

 

Is deburring really still this antiquated? Do I still need to create all the geometry to dodge walls and such? Or is there something better?  I was hoping there is something better, but digging around I am not seeing it. Can someone clarify there is something better or nope, same as 15 years+ ago?

Link to comment
Share on other sites
44 minutes ago, JParis said:

There are no specific deburring paths

That said, since there are no paths and what people want to do is all different, as mild or as wild it is on the user

True and thinking about it, lots of people use balls to deburr etc.

However, I'm specifically talking 2D contour chamfer using a 90degree spot drill - ie prismatic/plate parts

Link to comment
Share on other sites

Really going to come down to your parts, machines and requirements needed for the deburr. I have no issue letting a 800 run time part have 10 hours of deburr added to it on the machine while some companies have a complete melt down if the machine spends more than 12 seconds deburring anything on the machine. Throw together some example parts and file and then people can offer suggestions. Be good to know if you are looking for Chamfer tools, Ball endmills, Roto-Burr Tools or what you are thinking for tooling also.

  • Like 1
Link to comment
Share on other sites

I always try and take out the human work and add machine deburring as much as possible. 1/8, 1/4, 90 degree csinks/chamfer endmills. I was hoping there was a better way to dodge walls with out having to create offsetted geometry as much as possible. Doesnt take too long but if any changes happen then I am back to remaking paths for the deburring. This is an example of deburring needing to dodge walls. 

1-8 DEBURR.jpg

Link to comment
Share on other sites

For stuff like that 2D Chamfer all day....no offsetting lines

Set the upper edge, use the chamfer settings to a chamfer size, set the offset to drive the tool down away from the wall, then use lead in/lead out to control the ends.... 

 

JM2C :)

Link to comment
Share on other sites
1 hour ago, JParis said:

For stuff like that 2D Chamfer all day....no offsetting lines

Set the upper edge, use the chamfer settings to a chamfer size, set the offset to drive the tool down away from the wall, then use lead in/lead out to control the ends.... 

 

JM2C :)

+1 to this, that is how I would tackle a job like that too is with contour set to chamfer because then you don't need to offset that geometry that I see you created, another benefit by taking doing it in this manor is on a close wall like you have in that pic you could even use the Tip Offset setting for the chamfer toolpath to allow a higher contact point so you can allow the toolpath to cut with closer to the top of the chamfer mill which gets you further away from that wall instead of cutting with closer to the tip of the chamfer mill.

image.png

  • Like 1
Link to comment
Share on other sites

sometimes you need to run the part and see where the burrs show up, turning and milling based on tool path selection create different burrs in different areas.

I also use 3M coated brushes to run over the part to help deburr in a very fast manner

Link to comment
Share on other sites
23 hours ago, Matthew Hajicek™ - Conventus said:

It would be a nice feature to be able to add check surfaces to 2D Contour though; that would speed things up and take out any guesswork.

About 10 years ago I used Camworks inside SW. It had this, select and edge and you could pick walls to avoid. It was the only think I liked about that software to be honest.

Link to comment
Share on other sites

Mastercam does also, but you need to use 5 Axis Parallel and change the process to amount of cuts. Make it one and good to go. Many ways to do many things in any CAM Software up to each of us to learn what each one can do. Some Software has more ways and others have less, but at the end of the day how much of us really know what we are using 100%. 

  • Like 1
Link to comment
Share on other sites
53 minutes ago, 5th Axis CGI said:

... but at the end of the day how much of us really know what we are using 100%. 

I'd be amazed if the majority of us actually know or use 50% of the capability.

But +1 to the 2D chamfer path being stock aware. Be great to set the tool up and just say clear by 4thou and let it go.

Link to comment
Share on other sites
2 hours ago, 5th Axis CGI said:

Mastercam does also, but you need to use 5 Axis Parallel and change the process to amount of cuts. Make it one and good to go. Many ways to do many things in any CAM Software up to each of us to learn what each one can do. Some Software has more ways and others have less, but at the end of the day how much of us really know what we are using 100%. 

Ron, I wouldn't have thought directly to use parallel for deburring, but it makes sense, I use the moduleworks paths for a crap ton of simple stuff now as it gives you much more control using collision control.  Even if in 3-axis mode.  Sometimes makes for longer tool path creation time, but you typically get closer to what you were thinking with less effort.  Pretty delicate balance here sometimes.  But overall, you can save large percentages of run time on a 10 minute cycle time if you can keep the tool in cut start to finish.

Link to comment
Share on other sites
On 4/19/2017 at 7:40 AM, 5th Axis CGI said:

Mastercam does also, but you need to use 5 Axis Parallel and change the process to amount of cuts. Make it one and good to go. Many ways to do many things in any CAM Software up to each of us to learn what each one can do. Some Software has more ways and others have less, but at the end of the day how much of us really know what we are using 100%. 

 

Works great for fillets also. Parallel and Morph are my two goto paths.

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...