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:

Machine undercut with lolly-pop cutter


Mcam Nut
 Share

Recommended Posts

I am trying to finish a slight undercut on a surface and the operation wants to cut straight down the wall and wont allow me to under cut.  I am not using a stock model, just want to add a quick toolpath to the part.  I tried scallop, contour and hybrid, and all have similar results. on contour I clicked detect undercuts and it still wants to cut straight.

i use mcam 2019 because I am too lazy to update

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

Make sure you define a straight shank lollipop....tapered shanks don't work for undecutting

I did use straight shank

17 minutes ago, gcode said:

try old school waterline … and disable gouge checking

I just tried but cant find the gouge check in waterline

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

A file is going to make this easier...SFC and SFF will both accomplish it...likely need to see it to figure out what's happening

its been a while since i shared a file, its 25mb, can I share that?

7 minutes ago, crazy^millman said:

Surface Finish Contour. If you have the 5 axis then try Morph or Parallel to either curve or surface. 

Old School Surface Finish Contour? 

Thats the one i was trying to use but its not working 

Link to comment
Share on other sites
9 minutes ago, Mcam Nut said:

its been a while since i shared a file, its 25mb, can I share that?

Thats the one i was trying to use but its not working 

Strip the file down to just the few surfaces or area in question and the toolpath you are trying and share just that section. I can share a dropbox upload link that I can then post here for others to grab it from. 

Link to comment
Share on other sites

Use Flowline. Turn off all gouge checks.

Surface Finish Contour seems to be broken for Undercutting. I have used it successfully dozens of times in versions before 2017. I haven't had to do Undercutting since about X9.

I tried it just the other day in Mastercam 2020, and Surface Finish Contour was broken for doing this...

Link to comment
Share on other sites
13 minutes ago, Colin Gilchrist said:

Use Flowline. Turn off all gouge checks.

Surface Finish Contour seems to be broken for Undercutting. I have used it successfully dozens of times in versions before 2017. I haven't had to do Undercutting since about X9.

I tried it just the other day in Mastercam 2020, and Surface Finish Contour was broken for doing this...

Flowline is crashing my computer, for a simple operation this is being very frustrating

Link to comment
Share on other sites
16 minutes ago, Mcam Nut said:

its still not following the surfaces when i backplot.  it cuts the top rad fine, then just cuts a straight wall after the top rad

Okay now we are on to the real issue you are running into. I couldn't get Surface Finish Contour to work. 

Here is the file with Morph Added. 

Morph Between 2 Curves 3 Axis

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
7 minutes ago, gcode said:

Thought I was losing my mind

I used to do this all the time and couldn't make it work

I had the exact same feeling Tom. Something that I've done successfully, many, many times, and all of a sudden it just won't work no matter what options you throw at the toolpath.

Between this, the "trimming" debacle, and the Planes SNAFU, I'm getting a little gun-shy of Mastercam.

I hate saying that; as it has been such a great tool in my toolbox for so many years.

I really hope CNC Software can work some magic in their 2021 updates, because some of these issues are becoming deal-breakers for me...

Link to comment
Share on other sites
11 minutes ago, Colin Gilchrist said:

I had the exact same feeling Tom. Something that I've done successfully, many, many times, and all of a sudden it just won't work no matter what options you throw at the toolpath.

Between this, the "trimming" debacle, and the Planes SNAFU, I'm getting a little gun-shy of Mastercam.

I hate saying that; as it has been such a great tool in my toolbox for so many years.

I really hope CNC Software can work some magic in their 2021 updates, because some of these issues are becoming deal-breakers for me...

didn't there used to be a check box that told it not to gouge check.... and if you checked it the toolpath would machine undercuts... 

the gouge checking  was up to the programmer??

I remember doing 1.5" deep angled undercuts with a Ø6" wheel cutter with this toolpath in V9, easy as pie ????

Link to comment
Share on other sites
16 minutes ago, gcode said:

didn't there used to be a check box that told it not to gouge check.... and if you checked it the toolpath would machine undercuts... 

the gouge checking  was up to the programmer??

I remember doing 1.5" deep angled undercuts with a Ø6" wheel cutter with this toolpath in V9, easy as pie ????

Yes.

It seems to have been replaced with a 'detect undercuts' checkbox instead.

It doesn't matter if that checkbox is now enabled or disabled, the toolpath just will not drive an undercut surface, no matter what options I pick.

Link to comment
Share on other sites

I think it's working, it's just such a small undercut it's hard to see

I changed depth settings to Absolute relative to the center of the tool and made the tool shank the same diameter as the

shoulder.

If you backplot it and check  the X values you'll see every step down is a little bit bigger X value that the one before

 

gcode ucut.zip

  • Like 1
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...