Reference lines for dimensions – Fusion 360

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Reference lines for dimensions – Fusion 360

Home Forums CAD – Technical drawing & design Reference lines for dimensions – Fusion 360

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  • #812611
    John McCulla
    Participant
      @johnmcculla

      Hi all,

      I’ve been playing about in Fusion 360, trying to redo an old drawing used as teaching material on my course.

      I’ve modelled the part successfully, but I can’t find a way to include a reference line running through the hole centres in the final ‘Drawing’ section. I need this to show the 22.5 degree angle.

      Can anyone shed any light on this, or am I trying to use the wrong program?

      Screenshot 2025-08-15 at 16.56.31Screenshot 2025-08-15 at 22.12.34

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      #812618
      blowlamp
      Participant
        @blowlamp

        I don’t have Fusion 360 so I cant help you there, but what does the horizontal centre line reference to on the part, as It doesn’t seem to be parallel with either the upper or lower straight lines of the part as drawn in your second photo?

        I ask because my CAD finds an angle of 21.8 Degrees rather than the expected 22.5.

         

        Martin.

         

        22.5 Degree

        #812627
        JasonB
        Moderator
          @jasonb

          As a stand alone part it could just be drawn with teh three holes horizontally but that kind of defeats the object of repeating the exercise.

          I hardly ever use 2D in F360 but worked itout fairly quickly.

          1. To get the angled ctr line chose “centre line” from the geometry section and then click the two lines I have ringed in green which will put a ctr line between them

          2. Next select “centre mark” again from geometry and then click the 36mm circle(not the ctr as I have ringed) this will give the vertical and horizontal ctr lines.

          3. From the dimension drop down select “angular” and then click the angles and horizontal ctr lines you have just created and it gives the angle between.

          I drew it from the dimensions given and placed the two 8.7mm holes & 12mm radii at 22.5deg then the four straight edges were done as tangents and not drawn horizontally.

          f360 angle

          Measuring the angle that the two taperes meet at it is not 45deg as you would expect given the way the original drawing is laid out. But looking closely at that original drawing the top and bottom edges are not a good tangent to the 12R ends.  So should that non tangent be recreated on the new F360 model?

          If you actually take the dimension needed to get the part as dimensioned out of a rectangle it all becomes clear where the error is likely to have originated from. At 50.79mm I wonder if the drawing were originally imperial and they have just rounded what would have been a 1″ 25.4mm radius to the new metric 25mm

          not tangent 1

          not tangent

           

          #812630
          JasonB
          Moderator
            @jasonb

            Here is my initial sketch if that is of interest

            flange sketch

            #812633
            John McCulla
            Participant
              @johnmcculla

              PXL_20250816_074556875~2Thanks guys, I haven’t been as clear as I should have. I can get the reference line to appear in the sketch as Jason has displayed in the post above this, it’s in the final drawing page I’m wanting it to display. I suspect that it’s not possible because it’s not needed to create the part as such, but I thought I should check.

               

              #812634
              John McCulla
              Participant
                @johnmcculla

                I had noticed that the 22.5 degree angle was wrong, but I hadn’t figured out why, that’s some good detective work guys!

                #812641
                JasonB
                Moderator
                  @jasonb

                  John, You were clear enough. My first post is the 2D drawing and I give details of how to get the lines (geometry) you require to then add the 22.5deg dimension

                  #812648
                  Martin Connelly
                  Participant
                    @martinconnelly55370

                    I think it’s probable that this part was hand drawn and expected to be made out of 50mm wide bar stock by someone wanting to keep machining of the flat sides down to a minimum for whatever reason, possibly cost in a factory. Blending of the curves and straights was of secondary importance. We are spoilt because we have CAD and lots of time to do simple parts on relatively cheap machines with equally relatively cheap tooling. It’s an great example of how working practices have changed over the years.

                    Martin C

                    #812652
                    blowlamp
                    Participant
                      @blowlamp

                      This is what I get after correcting the angle to 22.5 Degrees whilst keeping the dimensions as drawn. It results in the 12mm rads having their centres relocated slightly away from the 8.7mm hole centres – as per the dimension in red.

                       

                      Martin.

                       

                      Screenshot 2025-08-16 110558

                      #812657
                      SillyOldDuffer
                      Moderator
                        @sillyoldduffer
                        On Martin Connelly Said:

                        I think it’s probable that this part was hand drawn and expected to be made out of 50mm wide bar stock by someone wanting to keep machining of the flat sides down to a minimum for whatever reason, possibly cost in a factory. …

                        Martin C

                        I agree Martin is probably right.  So also is Jason – the draughtsman made a mistake!

                        Just possibly though, maybe the drawing was tilted as an exercise just to extend the students skills, and not worked out fully.  The creator didn’t know his example would be tested by a CAD package that highlights issues humans might miss.

                        In my innocence, I would draw this with the centre line horizontal and do the sums later as necessary to make the item from bar stock.  Martin is smarter than me, spotting the thing is essentially 50mm.  Actually I make the distance between parallels to be 49.6694mm.  Not investigated yet why they aren’t exactly 50mm apart, in accord with the drawings largest diameter:

                        horiz

                        Anyway, to get the tilted version, I simply rotated the whole drawing by 22.5°.  Rotations are trivial in most CAD applications, but hard work on a mechanical drawing board!  But rotating by 22.5° reveals that the lower straight line is off-horizontal by 0.696°:

                        tilted

                        I no longer have F360, discarded in favour of SolidEdge, because AutoCAD altered the licence conditions and are able to enforce  new rules because the product has to phone home periodically.  SolidEdge is harder to learn, but it runs locally.  My examples are QCAD; no problem, Jason has answered John’s original F360 question.

                        Does this drawing being slightly faulty matter?   Not when making a few parts from it in my workshop, where only the hole sizes and coordinates are important, and could be gently bodged if need be.  More serious if the part is mass-produced as an interchangeable spare.  Fireworks if an engine builder orders 100,000 of them, and finds they don’t quite fit into a tight space on his engine…

                        Dave

                        #812660
                        JasonB
                        Moderator
                          @jasonb

                          It would be interesting to see the whole exercise and any other view of the part. Also what was the date of that eddition and the first eddition( imperial?). If imperial stock was still about then it would fit nicely in a bit of 2″ flat bar being 50.79mm wide.

                          Are the dots punch marks and the students expected to file all three holes to size?

                          #812668
                          JasonB
                          Moderator
                            @jasonb

                            If the rectangle in the original drawing is not a border but part of the item then it could be it should look like this cut from 100x 50 material and then the 22.5deg angle is correct if a mating flange needs to fix to it at that angle. If that flange were smaller overall then it would not matter if the drawn part did not have tangent features

                            rec flange

                            #812674
                            blowlamp
                            Participant
                              @blowlamp

                              If the rectangle constitutes part of the item, then by rights the overall length should be given in the measurements, along with the horizontal centre locatation of the large circle.

                               

                              Martin.

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