Learning CAD with Alibre Atom3D

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Learning CAD with Alibre Atom3D

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Viewing 25 posts - 276 through 300 (of 841 total)
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  • #382782
    David Jupp
    Participant
      @davidjupp51506

      Paul,

      In the copy of the article that I'm looking at ( a draft, so could have changed slightly for publication) constraints 1, 2 & 3 fix the base in the assembly workspace. Constraints 4 & 5 join the column to the base.

      I don't follow quite what you mean by 'cannot find Align 3' …

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      #382837
      Paul Abrams
      Participant
        @paulabrams18342

        Thanks David

        When fixing the base into the assembly workspace I can only find and fix constraints 1 and 2. Constraints 4 & 5 for fixing the column become 3 & 4.

        Is it possible that the base enters the workspace at zero height and therefore doesn't need constraining?

        Haven't tried it this morning but maybe if I tried moving the base upwards in the workspace before constraining then maybe I'll find the 3rd alignment?

        I'm out for the day but will try tomorrow. I'm liking the software but wish I could learn it faster – Wish I was born with a better brain!

        #382841
        JasonB
        Moderator
          @jasonb

          Paul,

          Constraint 1 sets the bases position to the XY plane (side to side)

          Constraint 2 sets the bases position to the YZ plane (front to back)

          Constraint 3 sets the bases position to the XY Plane ( up down)

          Depending on where you clicked when you inserted the part into the assembly screen it may well be sitting on the XY plane but is movable

          Step 3 is not really critical on a small assembly like this but worth getting into the habit of tying down your first part as when you come to have many more items in an assembly it will help a lot and you won't find previuosly placed parts moving to join a new part when you really want the new part to move to the main assembly.

          Edited By JasonB on 29/11/2018 08:59:38

          #382848
          Paul Abrams
          Participant
            @paulabrams18342

            Thanks Jason

            It is not having a second XY plane visually available which is causing the problem. No matter where I place the base in the window there is not a second XY plane available.

            As you say it is not critical so I shall move on!

            #382852
            JasonB
            Moderator
              @jasonb

              Paul, can you post a screen shot of what you have. It is also possible to select the bottom surface of the part and the plane to align those.

              It may be you don't have the planes and axis of the part showing, if not right click the part like I do in this video and select show reference geometry.  Note the reason it flipped sideways was due to me having the top surface selected (Blue) when I clicked the plane so it thought those were the two items I wanted to line up, simple undo got rid of that.

              Edited By JasonB on 29/11/2018 10:14:23

              Edited By JasonB on 29/11/2018 10:17:30

              #382860
              duncan webster 1
              Participant
                @duncanwebster1

                This might be complete tosh, or it might help. At first I had what I think might be Paul's problem, I found that I need to plonk the part away from the assembly frame of reference so that I can then differentiate between the XY plane of the assembly and the XY plane of the part. If they are too close you can't click one then the other.

                #382871
                JasonB
                Moderator
                  @jasonb

                  Certainly not tosh

                  If when you place the part you move the cursor to where the axis meet so it looks like this and click.

                  dsc03385.jpg

                  You will get all the part axis lined up with the assembly ones and no easy way to select either all you see is a slight change of colour and the lettering of each green axis. This is much like when sketching and you place say a circle on one of the axis, it will line itself up but won't have its position fully defined.

                  overlay.jpg

                  #382969
                  duncan webster 1
                  Participant
                    @duncanwebster1

                    Does the stricture on renaming apply also to moving files to a different directory?

                    #382970
                    JasonB
                    Moderator
                      @jasonb

                      I think that should be OK but if you have used those files in an assembly it will go looking for them in the original location.

                      #383010
                      David Jupp
                      Participant
                        @davidjupp51506

                        Duncan,

                        Always best to use Save As, there are probably exceptions where it doesn't matter (but very specific circumstances). Safer to just always use Save As.

                        #383011
                        JasonB
                        Moderator
                          @jasonb

                          David if it is best to "save as" rather than move to another directory, folder etc then how do you get on sharing Alibre files as they will not be in the same directory when opened on another computer?

                          I've not noticed problems opening others part files, only when opening an assembly where the file location of each part needs altering on the box that comes up.

                          #383021
                          Paul Abrams
                          Participant
                            @paulabrams18342

                            Thanks Jason & Duncan

                            Moved the body upwards and it showed the third XY plane so I'm OK with the problem now – Sorted

                            #383022
                            Emgee
                            Participant
                              @emgee
                              Posted by JasonB on 29/11/2018 11:47:36:

                              overlay.jpg

                              Hi Jason, I note on the above model you it appears you have drawn the sketch on the ZX plane and extruded on the XY plane.
                              Or you may have drawn the 1/2 section on the XY and rotated the shape to get the model. Is there a good reason for using the drawing plane chosen ?

                              The reason for asking is I have always drawn the sketch on the XY plane and extruded the model on the Z axis, this way it conforms to the axis planes on the milling machine and lathe.
                              If you are not assembling the parts does it matter which plane you start the sketch on ?

                              Emgee

                              Edited By Emgee on 30/11/2018 09:35:10

                              #383026
                              JasonB
                              Moderator
                                @jasonb

                                Emgee, if you have a look back at the first page you will see where I raised this point.

                                I tend to draw a part as you would see it in use so that base is drawn so it sits on a flat surface when I click the default isometric box rather than as it would be poking out of a chuck. Maybe it's my construction back ground but we always draw a building on its foundationswink 2 This also puts it the right way up when you come to do 2D drawings

                                I also find it makes looking for a part a lot easier if they are all saved the right way up, you don't have to look at the manes when the parts are easy to identify and they are also all in the right plane when it comes to assemble them.

                                 
                                It also puts them in what I would consider the right position for the default 2D  drawing layout, the engine base from the files in that video would look like this.
                                 
                                layout.jpg

                                Edited By JasonB on 30/11/2018 10:00:40

                                #383040
                                David Jupp
                                Participant
                                  @davidjupp51506

                                  Jason,

                                  The system can only get confused if you have files with duplicate IDs on your system. If you copy all the files (into e-mail, onto a memory stick, or some other method to share with others) they will only get the files you send, no rogue files that might exist in your system – hence their system can't get confused.

                                  For assemblies, or drawings along with the part(s), creating a 'Package' file is the simplest way to send everything to another user.

                                  Edited By David Jupp on 30/11/2018 11:08:50

                                  #383182
                                  John Barber 5
                                  Participant
                                    @johnbarber5

                                    Does it mean anything when a 2-D drawing dimension is shown in red? I added two further dimensions to an existing drawing and one came out red. I couldn't see any way to change the colour, but when I deleted the dimension and added it again, it appeared in black as normal.

                                    #383184
                                    David Jupp
                                    Participant
                                      @davidjupp51506

                                      John, a red dimension indicates that it has become 'disconnected' from the model. It may well still be correct, but probably won't update if you edit the model. You took the correct action by deleting and re-creating the dimension.

                                      #383191
                                      John Barber 5
                                      Participant
                                        @johnbarber5

                                        Many thanks, David.

                                        #383222
                                        M
                                        Participant
                                          @m

                                          Help, In the assembly part view I insert part but find it is 90 deg to what I what. How do you turn it. Is this possible/

                                          Regards

                                          Melv

                                          #383229
                                          JasonB
                                          Moderator
                                            @jasonb

                                            As you start to align one part with another, a plane or an axis it will move as you need maybe 90degrees or doing a complete 180degree flip.

                                            If that does not work post a screen shot of what you are trying to assemble.

                                            #383231
                                            David Jupp
                                            Participant
                                              @davidjupp51506

                                              You should also be able to 'free rotate' a part in the assembly space (though one person hasn't been able to get this to work). Hold down the shift key, then click & hold off-centre on the part and move the mouse. This should rotate the part – it isn't precise, but can help to get access to a particular face to apply a constraint.

                                              As Jason says – applying constraints is how you position parts in an assembly.

                                              #383251
                                              Emgee
                                              Participant
                                                @emgee

                                                Melv

                                                It may have been said but showing the reference planes, axis etc will assist you to reposition the part in an assembly.

                                                Emgee

                                                edited spelling error

                                                Edited By Emgee on 01/12/2018 20:02:30

                                                #383358
                                                duncan webster 1
                                                Participant
                                                  @duncanwebster1

                                                  This is beginning to 'do my head in' as my youngest would say. I'm trying to model a coupling rod, so I draw the boss at one end, then a vertical line from the centre 1/2" long and a horizontal line 5/32" long. Then mirror the horizontal about the vertical, and using the constraints icon, lock these 3 lines. All very nice so far, everything in black and no error messages

                                                  sk1.jpg

                                                  If I then offset the vertical line either side I get 2 red lines,

                                                  sk2.jpg

                                                  but no matter what it won't let me lock them, I get an error message

                                                  a constraint cannot be applies as it results in an over-constrained or inconsistent sketch.

                                                  My simple mind thinks that if the first vertical line is constrained, then creating an offset to a dimension results in another constrained line, but apparently not
                                                  If I then trim the outer curve inside the red lines and the red lines back to the outer curve, the outer curve which was constrained becomes unconstrained, and it won't let me lock it, same error message. If I try to make it coaxial, it says the constraint already exists.
                                                  This continues if I just ignore it and offset the vertical line by half the rod length and then mirror the boss about this new line, all of the new boss is unconstrained, but won't let me constrain it. If I carry on it does produce a convincing model, but #2 son is full of warnings about lack of constraints. Not finished yet, got to do the fluting, but it would be nice to know I'm not going to have to start again
                                                  sk3.jpg

                                                  but there are 3 red lines left which I can't get rid of.

                                                  HELPPPPPP

                                                   

                                                   

                                                   

                                                   

                                                   

                                                   

                                                   

                                                   

                                                  Edited By duncan webster on 02/12/2018 15:03:59

                                                  Edited By duncan webster on 02/12/2018 15:14:13

                                                  #383360
                                                  Neil Wyatt
                                                  Moderator
                                                    @neilwyatt

                                                    Not how I would have done it… I would have simply drawn a rectangle then dimensioned and constrained it to be in the right place.

                                                    But… it works for me. Are you starting you 'red' lines by dropping them down from the bar of the T?

                                                    duncans.jpg

                                                    #383364
                                                    David Jupp
                                                    Participant
                                                      @davidjupp51506

                                                      The verticals are not of defined length. An offset is a simple 'one time' operation which just creates the figure – it doesn't fix anything.

                                                      If working in fractional inches, why not set display units to fractional inches?

                                                      I would not personally mirror sketch content to make other half of the rod – instead form half the rod, then mirror the 3D feature. That all helps to keeps sketches simple – which is useful if you have to go back and edit.

                                                      I'd probably simplify sketches even further but have more individual features to build up the final rod.

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