Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Chamfer an Edge

B

burnme

New member
Hello all,

I am using Pro/manufacture in Wildfire 3.0 and I am trying to chamfer the edges of a part.

I do this on every part I program around all the edges to debur it before the operator removes it.

Is there an easier way than using trajectory milling.

I should be able to specify a tool and an edge and have the tool remove the same amount every time (.15mm)

Is there a way to make a sketched tool or a special sequence for this?

Burnme
 
burnme said:
....Is there an easier way than using trajectory milling.

I should be able to specify a tool and an edge and have the tool remove the same amount every time (.15mm)

Is there a way to make a sketched tool or a special sequence for this?...
Click to expand...





I think TRAJECTORY is the only option; at least that's what we're using for chamfering.


Set up a MILLING TOOL with 45deg side angle, .005 tip dia. and say. .250" length.


Set up (and save)parameter page (name itCHAMFERING or something equally descriptive) with e.g. .010" PROFILE offset and .010" AXIAL offset. We use 100IPM feedrate and 8500RPM for that. Lead-in and -out as you please, but Iskip that and plunge right in; its only a chamfer :)


For the actual tool we use 1/4" 6 (or 8) flute solid carbide chamfering tool with 90deg. tip. It looks like tiny countersink and works like a charm.


I hope it helps, once you save your tool and params, the rest is fairly simple.
 
Forget trajectory and create a volume over the top face of your job. Set the dept to .15mm & trim. If you then hide everything else you will see the thin track that the cutter will follow. To m/c, create a volume mill excluding any surfaces you don't want to chamfer.Then rather than draw a chamfer tool just call up a 3mm end mill and watch it run around all the edges. When on the machine put in a chamfer tool and move it onto the job with cutcom. It will then go around all edges so fast that sparks will fly!
 
Cambmac said:
Forget trajectory and create a volume over the top face of your job. Set the dept to .15mm & trim. If you then hide everything else you will see the thin track that the cutter will follow.
Click to expand...


Please correct me if I'm wrong, but that will work only if the part has the chamfer modelled around the edges? I guess some companies do that, but I haven't seen too many of those. Unless I didn't understand you... wouldn't be the first time I didn't understand things
smiley17.gif
smiley17.gif
smiley17.gif
smiley17.gif
smiley17.gif
 
No you do not need to model the chamfer, but I did forget mention that the param in volume m/c sequence should be set to profile.
 
Hello everyone


I am new to this site but have been using pro/man since 1993,only had 1 day of formal training so have been using alot of workarounds.I chamfer using the same volume or surface I created to mill with.I use a .250 dia. 90 deg. chamfer mill. I define the tool,telling pro its .080 dia.I then use an existing volume and offset axis in advanced parameters to achieve desired depth.Example:If I have machined a .500 deep pocket using volume I put in a -.46 axis offset just to break the edge.
 
Hi all deburrers!!


I know this is an old thread, but I thought i would share my method of deburring component edges. Firstly, I use copy & paste function to create a datum curve on the models chamfer feature. Then, I use the 2 axis trajectory sequence and define a chamfering or countersink cutter. In the sequence advanced parameters, specify a 'PERCENTAGE_LENGTH' value of between 0-1.This is the position along the angled portion of the cutter, ie 0.5=half distance.The system will calculate the datum curve contact point along the percentage length of the angled tool. Using this method, you do not need to cheat on the 'AXIS_SHIFT' or 'PROFILE_OFFSET' parameters.





You can also use the 2 axis trajectory sequence with a sketched tool. But instead of using the 'PERCENTAGE_LENGTH' parameter to chose the tool contact point, place the horizontal centerline of the sketch on your chosen distance along the tools angle. I use this method tochamfer the back of holes and the underside of flanges & floors.
smiley32.gif
 
How about this one?


I have large holes 160mm and I want to run a 45 degree chamfer tool 50mm diameter cutter, around each hole. I have 20 holes to do. This is the only way it can be done?
 
How about using a Profile sequence? This is pretty slick.

It requires that you have NO chamfers in the model, only sharp corners.

-Create a Profile sequence with a milling tool that has a 45deg angle.

-Set the parameters using PROF_STOCK_ALLOW and AXIS_SHIFT to develop the chamfer. The difference between the two will be the chamfer size. For example, if you have a 45deg milling cutter with a 0.100 CUTTER_DIAM, set the PROF_STOCK_ALLOW to .08 and AXIS_SHIFT to 0.110. This will yield a 0.030 chamfer, and shift the tool down so that it is not cutting right on the tip. Again, it is the difference that counts. You could leave the stock allowance at 0 and shift it by 0.030, but you would be cutting right at the tip - not good. Set LEAD_IN and LEAD_OUT to YES to get your CUTCOM going and apply a LEAD_RADIUS and TANGENT_LEAD_STEP value.

- For the profile surfaces, select all the vertical surfaces you want chamfered, and then the top surface.

- Go into CUSTOMIZE and delete the Automatic Cut so the Customize dialog is empty.

- From the pull-down, add an Automatic Cut.

- Select From-To Depth from the menu and select Done.

- Next, select From Depth and pick the top surf of the part. Then, select To Depth and again pick the same top surface of the part.

- Do a Done Cut and that's it! Easy edge breaks complete with lead in/outs, cutcom, and no trajectories.

Regards
Peter Brown
 
You must log in or register to reply here.

Sponsor

Articles From 3DCAD World

Back
Top