I am not sure how to go about creating this funny little part,
this is an operators compartment and the gap needs to be closed in so the operator can't slide his foot underneath the seat area, there is moving parts there. Where the work plane is, there is an existing floor there for the operators feet. I created a very bad, poorly designed part (L125100012.ipt)
Anybody know how to create this part so that it will fit exactly, into the assembly? I just played with the dimensions until it visually looked good. And I'm sure if I got it made as is, my welder/fitter would be able to make it work. I just don't like the sloppiness. I also can't constrain it because of the way I created it. Nothing lines up, no angle, faces or seams.
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Assuming the four corner points shown are co-planar (no, I haven't DL'ed the zip file), I would:
- make a workplane using the edges of the downward sloping and triangular pieces
- make work axes using the new workplane and each of the floor plane and wall plane
- start a new sketch on the new workplane
- project the two plane-defining edges and the two new work axes
- trim or overline to suit
- finish sketch
When modelling one's self into a corner, always let the existing geometry be your guide.
I did create all those points and axis' , it is hard to tell if it is co-planer from the pic, but it is not. That is the issue...
What I did was created a plane using p1, p2 and p3
created another plane using p2, p3 and p4
Then used some measurements from those planes and points to create this ugly part, the angles are off and the seams are inconsistant.
I am not familiar with surface modelling, and then thicken, but I'm sure there is a rock solid way to produce this part
The part that needs to seal this gap, doesn't have to be a curvy/flowing part, I would actually prefer a simpler, easy to produce part. A single bend from p2 to p3 should be able to produce something.
I am just not sure how to create a part such as this using work feautres such as points, and planes.
Thanks for any help!!
(I am searching this forum and youtube for help and tips aswell)
Ah, well... modify the procedure as follows:
- make the workplane as before
- make a new sketch on that plane
- project edges as before
- connect edge ends with a line to make a complete triangle.
- finish sketch and extrude
- make a new workplane using the new edge and the other workpoint
- make two axes using the newest workplane and each of the floor and wall surfaces
- make a new sketch using this latest workplane
- project the two work axes and the new part edge
- overline to suit
- finish sketch and extrude
- fillet/loft/revolve/whatever to clean up the joint
(- do yourself a favor and make a workplane that is normal to the "bend line" so that you can more easily make an auxilliary- type view to dimension the bend in the plate)
You may wish to also make a flat pattern. Easy peasy:
- make a copy of the part
- measure the two edge lengths of the second extrusion
- roll the EoP marker up to show just the first extrusion
- edit the sketch and add two more lines as measured previously
- finish the sketch
- edit the feature and add in the additional profile
- don't forget to save!
Sounds like you may have done something like this before...
I'll give it try tomorrow once i'm back into the office, just to clarify you making this as a normal part and not a sheet metal part? Cause I do need a flat pattern layout for cutting.
Yes, as a normal part. If you make the flat pattern part, you can perform a bend from a line located mid-plate. The resulting part should be a reasonably close match to the modelled version, or at least within your fabricator's fudge tolerance.
Here is a quick model which should give you some ideas how to model the part in Sheet Metal.
The files are in IV 2010 format.
Hmm, this is a bit over my head, as of right now, surface modelling is quite new to me. I actually can't follow how you created this. I will keep it and use it for reference though!! Thanks for you help!!
Actually, I just realized I didn't need to do any surface modelling, thanks to IgorMir files.
In my assembly, I created a new sheet metal part on one of the two planes created by the 4 points.
I created a sketch, connected p1, p2 and p3, finished sketch and used the face feature on that triangle
I created another sketch on the other plane, and connected p2, p3 and p4 to create the other half of my sheet metal component and used the face feature as well.
No here is where I realized something, when creating these 2 faces from different sketches, they automatically create a bend (based on sheet metal rule) at the joint. I was making this part ridiculously hard because I didn't know that. Because I was able to use project geometry to create the part, constraining the part to the assembly was very simple whihc was one of my main concerns.
Anyways, thanks for all the help and hopefully this helps others out!
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