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Saturday, September 3, 2011

Engine: 1 - piston pin and pin ring

Today I modelled two parts: pin connecting piston and conrod and ring locking axial move of that pin.

 Piston pin

Time to start FreeCAD...

FreeCAD start page is opened. Click on the Part Design link.


Now you are in Part Design Workbench. Click at the icon "Create a new Sketch" with circle and rectangle to start sketching.


You can see grid and two blue lines - 0X and 0Y axis. Red geometry icons became active, so click on rectangle icon and draw it. At this moment dimensions aren't important.


You have a rectangle. Try set up width: click on upper line and set constrain "Fix a length of a line...". Then you should see dimension. Double click on it and set to 60 millimetres. You can delete constraints by key [del]. In the left bottom corner there is "Task View" with list of used constraints.


Now we need smaller and bigger radius of our pin. Select one (bottom) point and use "Fix the vertical distance between two point or line ends". Only one point was selected, so it is distance from 0X axis.


Do exactly the same operation with second (upper) point and set dimensions to 6 and 11.


Now you can revolve sketch. Stop editing sketch by pressing "Close" button in "Task View" or icon "Close the editing of sketch". It is time to revolve by clicking icon "Revolve a selected sketch". Important: be sure that sketch is selected in "Tree view".


Houston, we have a problem. Sketch was revolved around Y-axis (coordinate system is in right bottom corner) but it should revolved around X-axis. Select Revolution in "Project view" and set values in "Data Tab":
x 1,00
y 0,00
z 0,00
Revolve should update - if not (bug in the application): activate sketch in "Tree view" (you can hide/unhide elements by [Space]) by double clicking on it and change something, eg. length constraint from 60 to 55. When you close editing sketch revolve will be updated.


Now you have pin. If you need chamfer edges, select tool "Chamfer the selected edges of the shape" (the revolution have to be selected before) and click on those edges.


List of selected edges are in "Task View"


Fillet works in a different way. Firstly you have to have selected edges, after clicking "Make fillet on an edge, face or body" fillets will be created. You can change radius of fillet in "Project view"-"Data" tab.
That's all, experiment yourself!

Download file.

Pin ring

Create new file, Select Part Design workbench and create new sketch. Try draw vertical line - you should see small icon nearly cursor. It is autoconstraining: line become vertical automatically. Next select bottom point (end of line) and use "Create a lock constraint on the selected item".


You can see two dimensions started from point (0,0). Set they to 0 - line would be our centreline.


Draw arc: first is centre point, next points will determine start and end angle. Try set up centre on bottom end of line if you have problem with autoconstraining, use "Create a coincident constraint..." (red point icon). Next use "Fix the radius..." to set radius = 11.5.


Fix the horizontal distance between start point and centreline to -1,20 - select point and line before.


Create next arc higher, put it centre at centreline by "Fix a point onto an object" constraint and set vertical distance to 1.3.


Connect arcs with polilines. Next constrain left side with distance and angle constraints.

Left and right points have different position - we need something like a mirror. You can use symmetry constraint: select left point, right point and centreline then use "Create an symmetry constraint..."


Draw two circles. Set position one of them by "Create a lock..." 9.20 vertical and -3 horizontal would be good. Use symmetry constraint, and "Create an equality constraint...". At the end set the radius to 1.


Our sketch is complete but we have to do one important thing. Our "centreline" actually is a normal line. To not collide with sketch shape during Pad centreline must be toggled to construction mode - please select icon line with red points and blue line.


Click "Close the editing of the sketch" and next click "pad" in "Task View". At the end set pad length to 1mm in "Task View".


You can add also some fillets.

Download file.
If you stuck somewhere during this tutorial you can download video.


 What can you do with this model? For example:
  • export as STEP file (select File-Export, part object have to be selected in Tree view),
  • create 2D views and save it as SVG file (you can use Inkscape to convert SVG to DXF, FreeCAD DXF-exporter is still buggy),
  • create a mesh.



Version of FreeCAD: 0.12 r4875 SVN

33 comments:

  1. Hi! Great tutorial! I'm just beginning with FreeCAD, and when doing this tutorial I receive an error:
    "Sketch with conflicting constraints
    Please remove at least one of the constraints (1, 2, 3, 5, 6, 7, 8, 13, 14, 15, 16, 21, 22, 23, 24, 25)" This appears in the console when I try to apply some symmetry constraints.
    Thanks!

    ReplyDelete
  2. Your sketch seems to be overconstrained. In thr left bottom corner you have constraints list. Delete one of more (simply pressing [del]). If it still doesn't work you found bug!

    Recent FreeCAD version shows degrees of freedom counter. It should be 0. If it is more than 0, the sketch is underconstrained - you have to add some constraints. If you get message "Sketch with conflicting constraints", sketch is overconstrained and you have to delete some constraints. I also recommend you watching http://www.youtube.com/watch?v=y6EeuBnlVUk

    ReplyDelete
  3. Thanks! Yes, I've been playing around with freecad these days and now I understand those concepts much better. Still, Symmetric constraint still give me some errors, but I suspect it's my fault :D

    ReplyDelete
  4. One of the best tutorial I have ever read : concise, full of different ressources not to get stuck and not boring. Many thanks.

    ReplyDelete
  5. anybody know how to move the constraints? like for example moving the "-1.20" up above the pin ring?

    ReplyDelete
  6. never mind i've figured it out, what i need to know now is how to get the second arc constraint closer to the top of the pin ring or does it matter?, i'll show you what i mean

    ReplyDelete
  7. Would you move second arc center point or only "point-on-line" constraint symbol? AFAIK you cannot grab and move contraints symbols...

    ReplyDelete
  8. This overconstrained condition seems to appear when the centerline (mirror line) is constrained using coincident constraints.

    As a workaround, this is not an issue.when its length and position are held using dimensional constraints.

    ReplyDelete
  9. CAD tutorial is one of the best technique to create and edit drafting and modeling concept for architecture or engineer designs. This type of tutorial is beneficial for students as well as developer to gain skill of CAD software.

    ReplyDelete
  10. Adrian, you might want to delete the previous comment which is obviously shameless spam. Or can you do that to Discus comments? It's a pity there's no dislike button.

    ReplyDelete
  11. I draw the shape (in Atocad style, with lines , circles & trim those ) & when I extruded the profile it didn' t result a plate form . why? what goes weong?

    ReplyDelete
  12. tis is the wrong pin

    ReplyDelete
  13. what was wrong in prewious prtScreen , pls help?

    ReplyDelete
  14. Use the Pad tool from Part Design workbench.

    ReplyDelete
  15. Is the example file of rthe ring actually fully constrained? I'm using the latest daily build in Ubuntu, and after toggling the center line to and from construction mode, I get identical behaviour to my own file, that is, 2 degrees of freedom, which relate to the length of said center line, and the position of the inside vertex below the hole.

    ReplyDelete
  16. Right, a constraint for the point should be added. Length constraint for the construction line is not necessary since it is used as symmetry axis.

    ReplyDelete
  17. Total cad newbie here :) I'm just trying your tutorial to get a bit of a feeling for freecad. When I add the symmetry constraint for an arc endpoint, I get a constraints conflict (though the constraint seems to work). On both arcs. I can't see how there is a conflict; do you have any idea what I could have done wrong? The other symmetry constraints don't cause conflicts.

    Using 0.12.5382

    ReplyDelete
  18. Could you try apply the symmetry as first constraint?
    Also, I would suggest try a newer version. FreeCAD 0.13 has an indicator for redutant (not conflicting) constraints and much better constraint solver.

    ReplyDelete
  19. Thanks, I've compiled from git, and now the symmetry constraints are OK. I was stuck with 2 degrees of freedom like Elmo below, and after some unsuccessful mucking around I'm stuck with 3 degrees now. It's pretty hard to find what those degrees are.. How can i find out?

    ReplyDelete
  20. Drag points one-by-one. I don't know better method.

    ReplyDelete
  21. Hey FreeCAD users,

    while i tried to get started with FreeCAD i have the problem, that i cann't edit measurement properties on my solids. I can scetch in free space and on faces but every time i try to extrude my scetches I cann't set the length property of me pad. I use FreeCAD on a Win8 64Bit machine.

    Please give me a hint where i can find help to solve this wiered problem.


    Thanks

    ReplyDelete
  22. Very nice tutorial. I am new to FreeCAD and been to learn a lot from your tutorial. I am having problem with chafer and fillet tools. I am getting error that says "No fillet possible on selected faces/edges". However, I am unable to find option to select faces or edges. Will be nice of you if you can tell where to find this options.


    I am using FreeCAD version 0.13 Ubuntu 10.04

    ReplyDelete
  23. I made this same mistake before finding this comment, but anyone who had used any other common CAD program could too.
    Why the **** is the actual extrusion function named 'Pad' and the cut/hole function named 'Pocket'? On top of that, the icon for the 'Extrude sketch' button that produces this infinitesimally thin silliness looks more like what the 'Pad' one *should* look like, while the 'Pad' button has an image that looks more like a block off-set from a sketch/plane.

    Crazy software designers, man... how hard is it to use standard terminology for a couple of the most core functions of this program?

    ReplyDelete
  24. FreeCAD uses CATIA terminology http://catiatutorial.blogspot.com/2008/07/making-pad-pocket-fillet-and-chamfer-in.html - one of the first and most powerful CAD systems.

    ReplyDelete
  25. That does explain it, but hardly anyone uses CATIA, and 'Extrude' & 'Cut' are far less ambiguous terms :(

    ReplyDelete
  26. Extrude is already a tool in the Part workbench, as is Cut. Hence the different names for their Part Design counterparts, which behave very differently.

    The lead dev is mainly inspired by CATIA, it's simple, either adapt or choose a different program. Insert rolling eyes here.

    ReplyDelete
  27. Hi! The video is dead. Could you refresh it?
    Thanks in advance.

    ReplyDelete
  28. It seems something with Ubuntu One is horribly broken now. I lost many my files (videos have been reduced to 1 byte!). I send report to Canonical and waiting for answer...

    ReplyDelete
  29. Question:
    Some my files have been "reduced to 1 byte" (from many megabytes). When I try download a file (eg. http://ubuntuone.com/5D0RvZchkCN4WEGQVrfinz ), it gives me "Could not download content from storage".


    Answer:
    A couple of months ago we had an incident in which contents of files
    stored in a particular storage server were deleted. Unfortunately, if
    you didn't have any back ups of this files, they are lost :/
    If you have a computer that hasn't synced in a long time it may have
    the older version.
    I truly apologise for the inconvenience this may cause :/

    Best regards,

    Julia


    TL;DR
    Canonical lost my files (and erased from HDD's due synchronization!) and I can do nothing...

    ReplyDelete
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    ReplyDelete
  31. Hi, thanks for your great tutorials. I'm successfully create piston pin and pin ring.

    ReplyDelete
  32. Try every point in sketch is connected/joined. To connecting the point, it should appear red dot near cursor. If not connected, select two point and use "create a coincident constraint on the selected item"

    ReplyDelete