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:

X6 3D chamfering with Lollipop, help needed


Matt@RFR
 Share

Recommended Posts

I've got a part that is driving me crazy trying to chamfer everything and am hoping you guys can help me with it.  My .mcx file is attached. 

 

The features in red are what need to be chamfered, on the ID of the part only.  Everything else is taken care of.  .005" chamfers.

 

post-64056-0-70766900-1440627423_thumb.jpg

 

I will be using an 1/8" lollipop for these features.  I realize a regular ball would do it but I need the lollipop in another area so it will already be in the spindle.   The customer estimates needing upwards of 500 / month of these parts, so cycle time is important.

 

I have tried 3D chamfer, pencil, flowline, scallop and blend, both with and without chamfers on the solid, with absolutely no luck.  Some came close but ended up looking just like I ran the cutter straight in to the hole, which I also tried.  If anything came close to working, I always ended up with the chamfer being way too uneven around the features.

 

I also tried all of the above toolpaths on a different plane to see if the vector made a difference, which it didn't. 

 

I would appreciate any help with this!  I've been flogging it for a couple days now and just need to get it ready for production.

BASE FINAL REV B.MCX-6

  • Like 1
Link to comment
Share on other sites

Easily done. I use a process I developed years ago where I drive the center tool using 3D Contour. I take and create a surface that represents the chamfer I am creating. I then offset that surface the radius of the tool I am using. I then use create curve flowline using number and 3 as the number. That gives you a centerline to drive the toolpath from that will chamfer the part like you are looking for in these complex shapes and features. Takes a little bit of modeling and sometimes you have to create fillets instead of chamfers, but either one will offset when used as surfaces. Do get the occasional mismatch that will require blended spline to join.

 

HTH(Hope that Helps)

  • Like 2
Link to comment
Share on other sites

I would try creating a .01 fillet on the "back side" of each feature. Use surface contour to use the back side of the lollipop mill to deburr, hopefully you have a 300 degree cutting edge. However, 5th axis' way would probably yield a faster more direct tool path. 

Link to comment
Share on other sites

Ron, your method made perfect sense and taught me several things, so thank you very much for that.   However, it's just not working.  When I offset the surfaces, they will either twist or fold on to themselves.  Failing to fix that, I used flowline curve on the good surfaces and used blended splines to connect the geometry I needed, but still end up with really funky shaped chamfers.  I'm sure I can eventually get what I need by manipulating the geometry by trial and error, but as you can imagine this is adding a huge amount of time to an otherwise simple part.

Link to comment
Share on other sites

Got it!  With all the messing around I had been doing, I inadvertantly moved my stock model down in Z .070" so nothing was making sense in verify.  I have no idea how I did that, but now that it's fixed, things are working nicely.

 

THANK YOU!

  • Like 1
Link to comment
Share on other sites

Ron you do not need to build flowline

way easier to use flowline rib cut option

 

~~~~~~~~~~~

Single pass flowline toolpaths

All of Mastercam's flowline toolpaths include a Rib cut option that lets you create a single cutting pass down the middle of the selected drive surfaces. This can be very useful for part features like ribs or flanges:

 

 

 

This option is available for the following toolpath types:

 

Surface rough flowline

 

Surface finish flowline

 

Multiaxis flowline

 

To create the single pass, select the drive geometry normally, then select the Rib cut option on the Flowline parameters tab:

 

 

 

Mastercam automatically disables other flowline parameters that do not apply when creating a single pass, such as stepover and the cut control distance.

 

Use the Resolution field to control how many "slices" Mastercam makes perpendicular to the cutting direction as it calculates the toolpath

 

 

HTH

  • Like 2
Link to comment
Share on other sites

Ron you do not need to build flowline

way easier to use flowline rib cut option

 

~~~~~~~~~~~

Single pass flowline toolpaths

All of Mastercam's flowline toolpaths include a Rib cut option that lets you create a single cutting pass down the middle of the selected drive surfaces. This can be very useful for part features like ribs or flanges:

 

 

 

This option is available for the following toolpath types:

 

Surface rough flowline

 

Surface finish flowline

 

Multiaxis flowline

 

To create the single pass, select the drive geometry normally, then select the Rib cut option on the Flowline parameters tab:

 

 

 

Mastercam automatically disables other flowline parameters that do not apply when creating a single pass, such as stepover and the cut control distance.

 

Use the Resolution field to control how many "slices" Mastercam makes perpendicular to the cutting direction as it calculates the toolpath

 

 

HTH

 

I had the best result with Flow 5-axis.  But, it only does less than half of the toolpath.  I must be missing something.  Lathe, face milling a slot into a conical surface, just trying to break the edge.  I had to model a radius around the edge to make it kind of work.  Any secrets here I don't know?

Link to comment
Share on other sites

I had the best result with Flow 5-axis.  But, it only does less than half of the toolpath.  I must be missing something.  Lathe, face milling a slot into a conical surface, just trying to break the edge.  I had to model a radius around the edge to make it kind of work.  Any secrets here I don't know?

I have seen the same thing why I use what I suggested works every time and I have the exact lead in/out controls I want as well. More than one way to accomplish something and the way I do it works for me, but is not the only way.

Link to comment
Share on other sites

Thanks Ron.  I also use brand x software and can pick a point on a sketched tool and drive that point on contact with the toolpath.  I wonder if there is a c-hook out there to do this or maybe adding capability on the next version release that we apparently all would like to see.  It is great when you can come up with your own way of doing it, but it is some extra leg work.  There is the 3D chamfer option, but it never works with the tool types that I'm using.

Link to comment
Share on other sites

Thanks Ron.  I also use brand x software and can pick a point on a sketched tool and drive that point on contact with the toolpath.  I wonder if there is a c-hook out there to do this or maybe adding capability on the next version release that we apparently all would like to see.  It is great when you can come up with your own way of doing it, but it is some extra leg work.  There is the 3D chamfer option, but it never works with the tool types that I'm using.

 

I use what I got and if that is what I have to do I do it. I care about making the best part possible. Yes it is some extra work than just clicking and edge and deburr this and take everything into account, but I just put my head down and do what I can to finish the job. I make my suggestions when I can and keep doing what I can.

 

Not sure where picking a point a tool would work on some of the shapes I cut? The point of contact with the tool is in constant flux and never the same place when coming up sharp edges to going into undercut conditions when the tool is tilted in a 3+1 or a 3+2 Axis operation. I used the 2D and 3D chamfer for a majority of the work, but when I need exact control I use the method I have laid out here. No guess, not mess just do a little leg work with CAD and good to go.

Link to comment
Share on other sites
  • 3 months later...

Back to this subject. I give Aaron Eberhard the MultiAxis Product Manager credit here for pointing me in this direction and working with me to see it through. We have a part I wanted to chamfer some pockets on the inside of a diameter. It is on a 32.200 ID bore and there are 24 pockets on the inside. He told me to try Parallel to Surface in the MultiAxis Solid/Surface Toolpaths. Use the inside diameter as the edit surface for the pattern and the chamfer as the drive surface. I wanted to keep the head at a 45 degree angle normal to the Z axis. I used Fixed angle to Axis and Z as the Axis and then 45 as the tilt angle. Linking needed a little tweaking not much. I got the perfect toolpath that I use to spend hours drawing all the geometry for like I explained here. need to go over different surfaces no problem let those be your Pattern surface. The only issue I might see is featuring, but with collision control I think you could control that.

 

I have created this sample file that I will leave up for 12 months. After 12 months if you come across this thread email me and I will be glad to email you the file.

 

https://www.dropbox.com/s/0iqxkri555mjv0d/5th%20Axis%20chamfer%20example.mcx-9?dl=0

 

There is a stock model without the radius on it. You can use that stock model for Verify and see how well this process works. You can also see a 200mm Power grip from Rego-Fix defined as holder used as well. I used a fillet to drive the chamfer, but the principle is the same. Also I could have picked all the surfaces to drive it verses use the Transform rotate and that would have kept the tool down while going around the inside, but just wanted to get the file out here for others to learn from it as well.

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...