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:

Is this possible with MC 2d?


CNCZACK
 Share

Recommended Posts

Ive only got basic MC with limited toolpath options.  We seem to be getting into more  dimensional parts. (which we are soon going to look into an upgrade). I just dont know where to begin with this part because of my limitations. The only question I have is, is it even possible to make this part in a 3 axis mill with my limited options I have with MC?  

 

level 1 has less fillets to maybe make the general shape. level 2 is the original with all the fillets. as you can see though there is a 15 degree angle that flows into a .5 radius 

3D PART..mcam

Link to comment
Share on other sites
32 minutes ago, CNCZACK said:

Ive only got basic MC with limited toolpath options.  We seem to be getting into more  dimensional parts. (which we are soon going to look into an upgrade). I just dont know where to begin with this part because of my limitations. The only question I have is, is it even possible to make this part in a 3 axis mill with my limited options I have with MC?  

 

level 1 has less fillets to maybe make the general shape. level 2 is the original with all the fillets. as you can see though there is a 15 degree angle that flows into a .5 radius 

3D PART..mcam

Mastercam 2022 Beta will give you the optirough toolpath in 2d, which will make things easier, this is an easy part on a 3d license.

Link to comment
Share on other sites

Sure it is with same CAD work. Figure out what size ball endmill you want to cut it with. Seeing how the bottom is .5 I would pick a 1" Ball endmill. Create a surface on the cone and then offset .5. Then use the create spline Flowline and make your geometry to drive a 3D contour toolpath. Then connect the Geometry and call it a day.  Now if you want to machine the original part then you would need to work with 1/4 ball endmill and then would need to offset the surface all the away around .125 and then can try flowline, but I would probably do a projected line at different depths and then work from there. Total time doing all that CAD work and making toolpath 4-6 hours. 3D license I could program the part complete in less than 20 minutes.

  • Like 1
Link to comment
Share on other sites
On 3/1/2021 at 4:59 PM, crazy^millman said:

Sure it is with same CAD work. Figure out what size ball endmill you want to cut it with. Seeing how the bottom is .5 I would pick a 1" Ball endmill. Create a surface on the cone and then offset .5. Then use the create spline Flowline and make your geometry to drive a 3D contour toolpath. Then connect the Geometry and call it a day.  Now if you want to machine the original part then you would need to work with 1/4 ball endmill and then would need to offset the surface all the away around .125 and then can try flowline, but I would probably do a projected line at different depths and then work from there. Total time doing all that CAD work and making toolpath 4-6 hours. 3D license I could program the part complete in less than 20 minutes.

Ok, im circling back around to this. I'm using a 3/4 ball mill. (only long enough ball we have). to create my surface would I pull the wire frame from the bowl (.5 rad) then move it .375 and then create my surface again, then use curve flowline to drive my 3d contour? 

Link to comment
Share on other sites
17 minutes ago, CNCZACK said:

Ok, im circling back around to this. I'm using a 3/4 ball mill. (only long enough ball we have). to create my surface would I pull the wire frame from the bowl (.5 rad) then move it .375 and then create my surface again, then use curve flowline to drive my 3d contour? 

Offset the surface the .375. Then create the geometry to drive the toolpath using the create/splines/flowline process to have something to drive the toolpath with. Use Off as the comp type and then in the Contour toolpath use incremental depth and -.375 deep. You have just now create a Mill Level 3 Toolpath using Geometry. You could rough each step with a Pocket toolpath also. Very old school, but how I use to do this in Mazatrol 25+ years ago with 3D shapes.

Link to comment
Share on other sites
38 minutes ago, CNCZACK said:

Ok, im circling back around to this. I'm using a 3/4 ball mill. (only long enough ball we have). to create my surface would I pull the wire frame from the bowl (.5 rad) then move it .375 and then create my surface again, then use curve flowline to drive my 3d contour? 

If you create a single surface you can use surface finish flowline, no need for all that extra work.

Link to comment
Share on other sites
1 minute ago, Thee Byte™ said:

If you create a single surface you can use surface finish flowline, no need for all that extra work.

Thats what im trying to work on now. I just didnt know if that was an option. Since I havent used surface stuff too much its a bit tedious finding what works with what as far as what line i can use to force it into one surface 

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

Thats what im trying to work on now. I just didnt know if that was an option. Since I havent used surface stuff too much its a bit tedious finding what works with what as far as what line i can use to force it into one surface 

Exactly why a Mill Level 3D or Level 3 License is needed here. Get the tools you need to do your job faster or spend the time using what you got. They are paying for it one way or another just not paying attention to the real cost. That wasted time doing all the this work is time you lost and time you cannot put on something else. Add up all that time in a year and think you can quickly see where the more capable seat is worth every penny.

  • Like 2
Link to comment
Share on other sites
1 minute ago, crazy^millman said:

Exactly why a Mill Level 3D or Level 3 License is needed here. Get the tools you need to do your job faster or spend the time using what you got. They are paying for it one way or another just not paying attention to the real cost. That wasted time doing all the this work is time you lost and time you cannot put on something else. Add up all that time in a year and think you can quickly see where the more capable seat is worth every penny.

Exactly. I think its needed at this point, its less of a "can you do it" vs what do you need to get this done. Some training with the new seat will be an obvious one 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...