17 Replies Latest reply on Jan 15, 2018 8:19 AM by Kevin Chandler

    Chamfers on Curved surfaces

    Tom Puttkammer

      i am trying to put a chamfer on a hole that is on a curved surface but i cant seem to get it to work with the chamfer tool.

      see below:

      this was made with a revolve (what i wanted)de.jpg

       

       

       

      this is what the chamfer tool does (not desired)de.jpg

       

      any way to make the chamfer like the top one in the tool?

        • Re: Chamfers on Curved surfaces
          John Stoltzfus

          In reality SW Chamfer Tool tries to stay perpendicular to the surface as it shows in the top picture, which could be right if the part was chamfered prior to forming. 

           

          To achieve the image in the bottom picture you would need to have a fixture to hold the pc at that angle to chamfer it.

           

          The question is - when will you be putting the chamfer in before or after bending?

          • Re: Chamfers on Curved surfaces
            Steve Calvert

            I think I've done this before but had to create a axis so that a plane could be set up where I wanted it.

             

            Steve C

            • Re: Chamfers on Curved surfaces
              John Stoltzfus

              Ok - just gave it a whirl

               

              You can use the chamfer tool, however you need to create workarounds...  What you need to do is get the hole edge flat and off the curve surface first, see below..

               

              • Re: Chamfers on Curved surfaces
                Paul Salvador

                Tom,.. in 2017,  you can use Face/Face but you'd need a hold line  (split line)... if you do not have 2017, you can do a Draft using parting line (off the split line)

                holdline.pngdrft 1.png.

                • Re: Chamfers on Curved surfaces
                  Kevin Chandler

                  Hello,

                   

                  Beat to fit, paint to match, but we got it (or we got somethin'):

                  I think a revolve is definitely the better route

                   

                  EDIT:

                  Since I have some legacy stuff leftover from other strategies, here is my workflow:

                  1. Create a plane normal to the section view we've all been using
                    1. This plane is offset to the right side of the hole axis by the chamfer radius
                    2. I recommend using equations
                  2. Create a boss extrude to add material across the width
                    1. convert entities on the upper arc
                    2. draw a line snapped to the edge of the new plane
                    3. Trim these two, leaving aec left of the line and line below the arc
                    4. Change the trimmed line to construction
                    5. Draw a horizontal, snapped to the line arc intersection
                    6. Complete the profile with vertical line to the leftmost endpoint
                    7. Extrude full width
                      You now have the deck to make the chamfer
                  3. You can use the deck for the hole wizard thru hole plane if it doesn't exist yet
                  4. Do a normal chamfer on the deck/hole edge, again, I'd reference the equation for this, too
                  5. Do a cut extrude to cut away the deck added above, leaving what remains of the chamfer
                    1. Convert entities including the right of the deck, and then extend the arc to the deck outline and trim
                    2. Cut across all

                   

                  I hope this helps.

                  Doesn't beat a revolve, but the workflow may be of use elsewhere.

                   

                  Cheers,

                   

                  Kevin

                  • Re: Chamfers on Curved surfaces
                    Kevin Chandler

                    Hello again,

                     

                    Please ignore my reply above, it is incorrect.

                    It sizes the countersink diameter on the right side, which being on the uphill side, prevents the flat head fastener from seating below the top surface on the downhill side.

                     

                    Below is an approach that correctly uses the downhill side to establish the csink diameter and it uses a hole wizard countersink.

                    I'm not in front of SW, so I can't put my model where my mouth is at the moment.

                     

                    But here is my proposed workflow:

                    1. Create a plane (which I'll call "Plane1") located at the future csink axis and perpendicular to the side of the part
                      1. Using the section views above, Plane1 should be at the axis and normal to the view
                    2. Create a plane ("Plane2") that's offset to Plane1
                      1. An exact offset amount doesn't matter, but locate Plane2 left of Plane1 and still crossing the top arc of the part
                    3. Create a Split Line>Intersection using the surface of the top arc and Plane2
                    4. Create a plane ("Plane3") that is parallel to the part's bottom face and maintains its location at the split line
                      1. In the plane command, select the split line first, then the bottom face
                      2. Plane3 should move up and down when you move Plane2 left or right with Plane3 maintaining coincidence with the split line
                        1. I used the split line method only to get Plane3's behavior, if there are other methods to the same end, fine
                    5. You can hide the 3 planes and the Split Line if you wish
                    6. Create a sketch on Plane3
                      1. Draw a circle, centered on the cink's future location
                      2. Relate the circle's OD coincident (or tangent?) to Plane2 so when Plane2 moves, the circle's radius is linked to the Plane2's offset
                        1. Optionally, you can equate these two in Manage Equations
                    7. Using the circle sketch, create a Cut Extrude, cutting upward
                      1. You can select Up to Next or Blind
                        1. If you choose Blind, you needn't worry whether this operation completely cuts above the sketch plane
                          1. Any remaining "overhang" on the uphill side is removed later. So any Blind value > zero works, we're just creating the surface for the Hole Wizard csink (which will be linked to the csink diameter for the exact amount of land required).
                    8. Start the Hole Wizard on the cut extrude face (or Plane3) and create a countersink for the appropriate fastener, located on the center of the cut extrude circle
                      1. Select custom sizing and we'll accept what's there for now, so click the green check
                    9. In Manage Equations, link Plane2's offset to the countersink's diameter dimension divided by 2
                    10. Select the conic face of the csink and start the Offset Surface command.
                      1. Enter zero for the offset amount and click the green check
                    11. Start the Extend Surface command and click the top edge of the offset surface
                      1. The resultant extended surface must always be above the top arc face on the uphill side, so either enter a blind value large enough for future part changes or create another plane that is always above the part and select up to surface for the end condition
                      2. Select "same surface" for the extension type and click done
                    12. Start the Cut with Surface command select the extended surface as the cutter. Click Flip cut if the wrong things disappear
                    13. Hide the extended surface
                    14. Modify the countersink in the wizard to suit, everything should tag along

                     

                    Hole wizard bennies over other methods:

                      1. All csink dims are now located in one spot that every hole wizard devotee is used to
                        1. Allows for quick review of remaining thru hole material as you adjust things
                        2. Allows for quick changes since you're going to have to determine min/max (by altering the csink diamter/head offset) for the drawing tolerance (preferably on the section's height dim, see caveat below)
                      2. The tree indicates the csink's fastener size so any mating tapped hole mismatch is more apparent and may be more likely spotted in a design review instead of at assembly or by the customer
                      3. You can add head offset in straight dimensions and let SW figure out the trig
                        1. Create a test assembly with this part and a McMaster flat head model
                      4. You can use the hole callout and with one click have all of the data already linked, unlike what you would otherwise have to cobble up to get the equivalent
                      5. You can readily change to any size flat head and jump between inch and metric (for this part or a future one derived from this one)
                        1. This includes the head angles: since chamfer defaults to 45° (which is a default to metric), there will be extra futzin' for 82° and 100°
                          1. And no indication of a mismatch until the customer tells you
                        2. Unlike separate ops, or revolve cut sketch, by changing inch/metric you automatically get the right head angle
                          1. Toggling between 82° and 100° to fix the wrong choice (as Kevin sometime does), is a quick correction
                      6. For the same size flat head, you can readily add more csinks:
                        1. In the cut extrude, add more patterned/mirror entities/equal circles to the sketch
                        2. In the csink wizard, add points to the centers of the new circles
                        3. Zero offset/extend the new csinks
                        4. Cut with surface the new extended surfaces
                      7. With multiple csinks in the same wizard op, your csink count is automatically adjusted in the callout

                     

                    Drawing caveat:

                      1. Being a hole wizard thing, you can create its hole callout, but the csink diameter is only valid at the one point on the downhill side, on the axis.
                      2. Since csinks are tough to measure regardless, I suggest creating a section view (like the above) and adding a thickness dimension (part bottom to low csink diameter point) since this can be measured (and toleranced).
                        1. If you do add this dim, either the diameter portion of the callout is a reference or the added dim is (I'd vote callout diameter is the reference)

                     

                    I hope this helps.

                     

                    Cheers,

                     

                    Kevin

                    • Re: Chamfers on Curved surfaces
                      Kevin Chandler

                      Hello,

                       

                      Here is the model for the above text (you can't hide the split line BTW):

                      M3 csink:

                      1/4" csink (only change was to the hole wizard csink size & metric to inch)

                      I've attached the part for those who may be interested.

                       

                      Cheers,

                       

                      Kevin