bearracecars Posted November 7, 2011 Share Posted November 7, 2011 Hi all! I'm excited I found cadtutor and this is my first post. Over the years Ive used cnczone but the autodesk forum seems to be dead unless you need a autocad to gcode macro. Can't even upload a .ipt extension. I'm a newbie to inventor 2011. I've used autocad almost daily since 2005. I am seeing a need for me to move onto the paramatric modeling side of cad. Please remember that i'm very new to this and i know that i'm am probably doing this backwards. I drew this part in an assembly by extruding the base then extruding the sides with notches to fit around tubing that is the assembly. I was thinking that i could just take that part, convert to sm then unfold for a flat pattern. So you know where i'm going? I can't unfold it. I did go into the sm defaults and set my material thickness. Still not sure if i did that right also. What would the proper way be to create a sm part like this? I also have included the assembly file that the part was created in. Thank you for the help. Bear side wheel cover.ipt frame assembly.zip Quote Link to comment Share on other sites More sharing options...
kencaz Posted November 7, 2011 Share Posted November 7, 2011 First rule in uploading assemblies is include the part files... Quote Link to comment Share on other sites More sharing options...
bearracecars Posted November 7, 2011 Author Share Posted November 7, 2011 Parts are all drawn in assembly. I haven't saved parts individually out of assembly. The part file that is there is the first one i started working on. Like I said I'm new at this trying to train myself. So please explain! Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 There are no bends in your part? Sketch1 has too more dimensions than required. Sketch2 is unconstrained. Sketch3 is not needed. You might read this document while I work up a solution to your part. http://home.pct.edu/~jmather/skillsusa%20university.pdf Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 These are the only dimensions needed to fully constrain this area of the sketch (use Symmetry, Equal =, Coincident constraints). Did you intend this .015 offset? Is your design intent for the blue arc to also be offset .015 bigger than the green projected circle? Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 These are some "oddball" angles. Are these really what you want? Is width and height the controlling design intent dimensions or the angles? Quote Link to comment Share on other sites More sharing options...
bearracecars Posted November 7, 2011 Author Share Posted November 7, 2011 Thank you Dr.Mather. Dimensions in Sketch 1 where done with Auto Dimension button. I seem to have problems finding the missing dimensions to fully constrain sketches sometimes. I have since constrained sketch 2. Quote Link to comment Share on other sites More sharing options...
bearracecars Posted November 7, 2011 Author Share Posted November 7, 2011 These are the only dimensions needed to fully constrain this area of the sketch (use Symmetry, Equal =, Coincident constraints).Did you intend this .015 offset? Is your design intent for the blue arc to also be offset .015 bigger than the green projected circle? No I didn't intend for the .015 offset. How did you get that dimension. I just tried to find the .015 and i cant get it to show. Design intent is for the for blue arc to be same as projected circle. Can i see a pic of the contraints you used? Quote Link to comment Share on other sites More sharing options...
bearracecars Posted November 7, 2011 Author Share Posted November 7, 2011 These are some "oddball" angles. Are these really what you want? Is width and height the controlling design intent dimensions or the angles? Yes, the width and height are controlling those angles. I also don't like it when "oddball angles, lengths, etc." are used. One thing that I've been thinking was, could i have just drawn the face and converted that to sheet metal? Then used the sheet metal tools to create the flanges? After that project the cuts from the tubing to the flanges? Quote Link to comment Share on other sites More sharing options...
bearracecars Posted November 7, 2011 Author Share Posted November 7, 2011 No I didn't intend for the .015 offset. How did you get that dimension. I just tried to find the .015 and i cant get it to show. Never mind, I just found it. Its the bottom to center of circle. Didn't intend for it, but its a non issue with final outcome of part. Its going to be plasma cut when finished. So tolerances will only be as good as that anyway. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 Because you have some bends going through these cuts - some special considerations will need to be made. Let me know when you are ready to work through this step-by-step (I don't have 2011 - so you will have to follow pictures and written instructions). Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 I see you are here - so I'm going to give a suggested solution (I don't like that this part is not symmetrical about the origin, and I would not suggest that a beginner use Adaptive techniques (the red blue arrows) but I'll ignore those problems). Create a construction centerline through the middle of Sketch1 as partially shown in my previous posts. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 Delete Extrusion 3, including the sketch. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 Delete Extrusion 2, but not the sketch (uncheck Consumed Sketches). Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 Delete Extrusion1 but not the sketch and not the dependent feature. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 Drag the red End of Part Marker in the browser above Sketch2 to hide it for now. Right click on Sketch 1 and Hide Dimensions for clarity. Create a WorkPlane by selecting the construcion centerline in Sketch1 and the XY-Plane in the browser. Click OK Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 Create a Boundary Patch surface using Sketch1 as shown. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 Pull down the EOP below sketch2. Edit Sketch2 Delete the extraneous point shown and delete all sketch geometry below the boundary patch as shown. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 You will see a pink dot (sick geometry) remaining on each arc. Right click on these dots and select Break Link (your screen will look slightly different than mine as I'm using 2012). Quote Link to comment Share on other sites More sharing options...
JD Mather Posted November 7, 2011 Share Posted November 7, 2011 Project Geometry the edge of the Boundary Patch and add dimension shown. Quote Link to comment Share on other sites More sharing options...
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