JD Mather Posted March 7, 2013 Share Posted March 7, 2013 A couple of tips - I'm not sure you want those lines connected as when you put the frame members in there they will require more complex intersecting trims. If you examine the skeleton I posted I left half the distance on each side for the size of the frame member so that they won't intersect rather than connecting the lines directly. Also, If you Project Geometry endpoint from one sketch to another - you should need only one 3" dimension on each end, and on the second end edit the dimension and pick the first dimension. This will make the second one a function of the first. Then end result - if you decide you need to change to say 4" there is only one dimension that needs to be changed to update the entire assembly. Quote Link to comment Share on other sites More sharing options...
trussman Posted March 7, 2013 Author Share Posted March 7, 2013 If you examine the skeleton I posted I left half the distance on each side for the size of the frame member so that they won't intersect rather than connecting the lines directly. The above quote confuses me I cannot see any of thew lines in that crane skeletal drawing thats not connected but I do see that your straight lines are yellow instead of the same color as the bracing or cross members not sure how or why this is. Also, If you Project Geometry endpoint from one sketch to another - you should need only one 3" dimension on each end, and on the second end edit the dimension and pick the first dimension. This will make the second one a function of the first. Then end result - if you decide you need to change to say 4" there is only one dimension that needs to be changed to update the entire assembly. You totally lost me here Quote Link to comment Share on other sites More sharing options...
trussman Posted March 7, 2013 Author Share Posted March 7, 2013 If you examine the skeleton I posted I left half the distance on each side for the size of the frame member so that they won't intersect rather than connecting the lines directly. Ah I see know what you are talking about. So do I need to draw construction lines for both the vertical frame members and the cross bracing in my sketch? If so then that brings me to the question of my material spec because I want to use a diameter that is different to what inventor is giving I am wanting to use 1 3/4" tubing with a .125 to .250 wall thickness. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 7, 2013 Share Posted March 7, 2013 If I came to a point these two members would intersec each other with a more complex trim. You can set offset from the red line when creating the frame member, but when there are compound angles involved the offset can get tricky so it is easier account for this in the skeleton. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 7, 2013 Share Posted March 7, 2013 I am wanting to use 1 3/4" tubing with a .125 to .250 wall thickness. You can add your own sizes\materials to the library. I don't do it often enough that I remember the steps - I have to follow the WikiHelp every time I do it. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 7, 2013 Share Posted March 7, 2013 You are doing too much work. In your Sketch1 you only need one dimension (unless there is a chance that this might be edited to be rectangular rather than square). You do not need centering dimensions if you use the CenterPoint Rectangle or the Polygon tool. Note that I set the two sides to equal. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 7, 2013 Share Posted March 7, 2013 Sketch2 isn't needed but if you are going to use it, use it to control the Extrusion distance by selecting the dimension. (I often control LWH like this with sketches as it is easy to double click the dimension and edit.) Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 7, 2013 Share Posted March 7, 2013 Work Plane1 isn't needed unless the apex is different size than the base as in my Lofted Crane Boom example. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 7, 2013 Share Posted March 7, 2013 Sketch10 wasn't needed. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 7, 2013 Share Posted March 7, 2013 Make one dimension a function of another by simply clicking on it. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 7, 2013 Share Posted March 7, 2013 Use Project Geometry (in this case a point) from one sketch to another. By doing this I don't need another 3" dimension. One 3" dimensions controls all locations. (see attached ipt file - Note no dimensions in Sketch4 of my file). Box Truss.ipt Quote Link to comment Share on other sites More sharing options...
trussman Posted March 7, 2013 Author Share Posted March 7, 2013 If I came to a point these two members would intersec each other with a more complex trim.You can set offset from the red line when creating the frame member, but when there are compound angles involved the offset can get tricky so it is easier account for this in the skeleton. [ATTACH=CONFIG]40700[/ATTACH] Ah I get what you are meaning now, but what do I do with the parts that are on inside of the straight tubes if you look at the top view after adding the pipe the cross bars show up inside them or does this matter? You are doing too much work.In your Sketch1 you only need one dimension (unless there is a chance that this might be edited to be rectangular rather than square). You do not need centering dimensions if you use the CenterPoint Rectangle or the Polygon tool. Note that I set the two sides to equal. [ATTACH=CONFIG]40701[/ATTACH] Understand that it will make life easier. I did not know that there was a center point option for those I was following a guide that said to do so for easiness. Sketch2 isn't needed but if you are going to use it, use it to control the Extrusion distance by selecting the dimension.(I often control LWH like this with sketches as it is easy to double click the dimension and edit.) [ATTACH=CONFIG]40702[/ATTACH] I was using it for the extrusion distance. Work Plane1 isn't needed unless the apex is different size than the base as in my Lofted Crane Boom example. Ok I knew I didn't need it after I placed it there I just forgot to remove it. Sketch10 wasn't needed. I dont see a Sketch10 on mine Use Project Geometry (in this case a point) from one sketch to another.By doing this I don't need another 3" dimension. One 3" dimensions controls all locations. (see attached ipt file - Note no dimensions in Sketch4 of my file). [ATTACH=CONFIG]40704[/ATTACH] I will try this out. Again thank you Quote Link to comment Share on other sites More sharing options...
trussman Posted March 8, 2013 Author Share Posted March 8, 2013 If I came to a point these two members would intersec each other with a more complex trim.You can set offset from the red line when creating the frame member, but when there are compound angles involved the offset can get tricky so it is easier account for this in the skeleton. [ATTACH=CONFIG]40700[/ATTACH] Wow that was alot of work unless I am doing it wrong I have uploaded what I did to see if I am understanding this correctly or not Sketch2 isn't needed but if you are going to use it, use it to control the Extrusion distance by selecting the dimension.(I often control LWH like this with sketches as it is easy to double click the dimension and edit.) [ATTACH=CONFIG]40702[/ATTACH] I also tried to follow what you was saying here, I did away with sketch 2 and simply selected how much to extrude while extruding I think this is what you was meaning. well here is what I did see if I am following you or not [ATTACH]40713[/ATTACH] Quote Link to comment Share on other sites More sharing options...
JD Mather Posted March 8, 2013 Share Posted March 8, 2013 ...but what do I do with the parts that are on inside of the straight tubes if you look at the top view after adding the pipe the cross bars Trim them. There are at least three or four options for trimming/extending/mitering depending on the need. I think I used Trim to Frame) planar face in this case, but I don't have Inventor up at the moment to check the terminology. These editing tools are on the Frame Generator tab. In some cases trimming (especially on some curved (bent) pipes) requires a special trick. If you run into something you can trim - as questions. A may or may not be here for a few days. Quote Link to comment Share on other sites More sharing options...
trussman Posted March 8, 2013 Author Share Posted March 8, 2013 ok for some reason I am not able to project geometry to the sides I know your not on here for a few days so I will leave this question open till you get back or someone else can answer Quote Link to comment Share on other sites More sharing options...
trussman Posted March 13, 2013 Author Share Posted March 13, 2013 Use Project Geometry (in this case a point) from one sketch to another.By doing this I don't need another 3" dimension. One 3" dimensions controls all locations. (see attached ipt file - Note no dimensions in Sketch4 of my file). [ATTACH=CONFIG]40704[/ATTACH] OK I must be misunderstanding you here when you are projecting geometry I was thinking you were talking about the placement of my lines in the sketch. Quote Link to comment Share on other sites More sharing options...
trussman Posted March 13, 2013 Author Share Posted March 13, 2013 OK I have a completed box truss now both the sketch and the frame generated assembly I wanted to run a frame analysis and not sure what I did wrong with it but one side of the truss is weaker than the other side or so says the frame analysis. I am going to research the frame analysis now to figure out if I did something wrong on setup of it or if I have something configured wrong with the frame itself. Here is the files I want to test the structure in to separate directions of gravity pulls so I ran 2 separate simulations with the 2 different directions of gravity which is horizontal and vertical. Quote Link to comment Share on other sites More sharing options...
Recommended Posts
Join the conversation
You can post now and register later. If you have an account, sign in now to post with your account.
Note: Your post will require moderator approval before it will be visible.