I am using Inventor Professional 2011.
I have a series of points that I've placed along a sloped line in a 3D Sketch. However, if I delete one of the points, all the points that have been created are erased as well. I found a way to get around it (remove the constraints of the point I'm trying to delete and then delete the point). However, if I want to delete multiple points, the solution I have would take up some time.
I don't want to create a rectangular pattern in a 2D sketch because, when the line changes slope, the pattern doesn't seem to recognize the new slope direction and the points appear offset from the new sloped line.
Is there a way I can get create some semblance of a pattern in 3D sketch and also have the ability to delete individual points within a series of created points?
Thanks in advance for your help!
The goal is to create roof stiffeners (channels) for a 12' x 42'-6" building module using the frame generator. I'm trying to make the wireframe as easily editable as possible so we can make future edits when creating different size modules.
The wireframe consists of 3D & 2D sketches, but most of the wireframe is in a 3D sketch. My plan of action is to create multiple points along the sloped construction line (indicating the roof slope) and project that geometry from a 3D sketch onto a 2D sketch. I'll use the point to point tool in generating the channels for the roof stiffeners. I don't use lines to create the stiffeners because when I generate the channels using the line placement, the side face of the channels are angled perpendicular to the slope of the roof instead of being vertical.
Although creating the points using a rectangular pattern in a 2D sketch seemed like the best option for creating those points, the pattern failed when I lengthened the wireframe. Although I used the slope of the roof for the pattern direction, when I lengthened the wireframe, the points were offset from the updated roof slope. It were as if the rectangular pattern only recognized the direction of the old slope, instead of the line itself.
Part 1 shows the entire module. Part 1_2 shows a close-up of the points I'm creating in a 3D sketch.
I hope this is the information you needed. Thanks for looking into this!
I've never been a fan of patterning in sketches, they never seem to work out and if you have a featured based on a pattern, as soon as the pattern changes the feature fails. It usually seems better to pattern at the feature or part level.
Here is a trick for aligining frame generator features to geometery:
Don't forget that, even if you want to create your frames by points, the pionts can be the end of a line. So you can still use your lines as part of the master sketch if that makes your geometry more stable.
If your design will take it, I recommend creating the first rail with the frame generator, and then patterning the rail in the assembly. You can Link the parameters from the assembly to the part file, and then use a formula to make sure that the pattern updates when the master file does.
Let me know if that helped!
Here's what I did:
Created new assembly>inserted part (the wireframe)>used the frame generator to create one of the roof stiffeners.
Using the rectangular pattern in the assembly, I selected the roof stiffener. However, when I selected the roof slope (in the 3D sketch) to determine the direction of my pattern, I couldn't select the line. In fact, none of the individual lines in the wireframe could be selected. Would you know why the pattern won't recognize the wireframe? Perhaps this calls for another post...
Hmm, maybe you need to use the frame itself to give the pattern direction. Other than that, try creating so work Axis in the part file, and then the assembly file.
I'm sure that you will work it out!
I did as you suggested and it works. It seems the 3D sketch (on the assembly level) isn't selectable in most cases (other than in creating a frame generated part). If I run my cursor over the 3d sketch in the assembly design window, the part doesn't highlight unless I run my cursor over something that was created using a 2D sketch. I've seen another posting of someone having a similar problem. Frustrating!
Do you know if Inventor 2012 has this problem?
Rectangular patterns must be created using an 'Edge or work Axis':
I can report that I couldn't pattern a part in an assembly using 2D or 3D sketch geometry from another part as the reference.
I could use edges and axis from another part however - as described in the help.
Is that helpful?
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