Hello! Im making a roof for this automower garage. The roof is going to work as a service hatch that can be opened from the front(the wall in the far left in the image below) and fixed in the garage backpart. The hatch/roof will have an incline and im trying to make the roof with shapes as seen in the image. Ive tried using loft from the front face of the roof to a sketch in the (approx) middle of the garage(see image below). Later the plan is that the roof/hatch will then continue from the sketch to the back using an extrude without incline. This is how it looks with loft:
From this loft path it looks like it might work, but Solid Edge does not understand exactly what i want. Here is how it turns out:
I want the protrusion to follow the red lines (that ive added in paint). As you can see, the loft creates unwanted shapes (see red arrows).
Ive also tried splitting the two top parts of the roof off(with sketch) to loft the different shapes seperate. But when i tried this I cant even select the sketch...
I realize Im surely not making this easy for myself but I dont know how to make this roof, do you guys have any tips for me?
NOTE: When the hatch is finished its supposed to connect with the garage side walls aswell, so if the top roof is finished i intend to:
* extrude downwards from the roof to the wall
* cut out the garage so that only the roof/hatch remains
* save part as roof and assemble them later
I bet there is an easier way to do this aswell, any tips?
Thanks alot for any help!
Hello Chris and thanks for the reply!
The two sketches had the same number of vertices. Ok I will try bluesurf with thickening next time and see how that turns out.
Yes I used include on the second sketch with extra lines, could that be the problem?
I solved this problem myself by splitting up the loft into three separate loft commands for the three rectangles that makes the two sketches. This worked and gave me the result I wanted.
The connection points between the extra lines count as vertices - even if the lines are co-linear. Go back into the second sketch and delete the extra lines. Close the gaps by extending the remaining lines and you will solve the problem. There is nothing wrong with using the include command but you need to be aware that it will generate many line segments because it is projecting the source geometry onto the sketch plane and it will capture every single line - even if they are co-linear. Therefore you need to clean up the resulting sketch geometry afterwards to get rid of the extra line segments - particularly if you are doing lofts or bluesurfs.