I am attempting to use the loft feature to create a surface between two pieces of projected 3D geometry. I have never used the loft feature before so its very possible I am making a simple mistake. I am aware that using projected geometry is not the preffered method of doing things but to try and re-draw, or even trace over projected construction lines would be difficult given the geometry of this part.
The reason I need this surface lofted between the two is that I need to exagerate the anlge on this piece, then I will be printing a plug to use for hydroforming the part.
Any help is greatly appreciated, Thanks for you time.
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Inventor 2010...? Do you have anything newer?
The problem is 3D Sketch6 - notice how it's broken into odd segments? It can be lofted, but needs a bit of help in the form of a better surface edge. Have a look at this - it's easier than typing. No point me sending you the part if you're using 2010 sorry
I have a copy of a student version of 2014 on my school laptop, however on my PC at work I only have 2010.
Here is what I have so far. I still need to fill the area between the surfaces with a solid. I have tried using sculpt and loft to acomplish this with out any luck. What is the correct method?
If you notice the area around the flat surface with the D-shaped features you can see I offset the flat surface by .075. My plan is to after I have the solid use the fillet command to add radi and smooth that transition out. Will that work? Is there a better way to accomplish that?
Thanks, your video was very helpful.
@jeregonn wrote:
Is there a better way to accomplish that?
I would
1. move the body to the origin
2. remodel it in Inventor from scratch (this will be a bit of work without the dimensions - can you get a drawing from the source?)
It took me about 4 hrs to remodel the part from scratch. (would have taken about 30-minutes with a dimensioned drawing)
@jeregonn wrote:
My plan is to after I have the solid use the fillet command to add radi and smooth that transition out. Will that work? Is there a better way to accomplish that?
If you continue down the path you are on - I would replace the Lofted surface with a boundary Patch tangent to the fillets.
The drawing for this part is "Reduced Dimension." It has no useful dimensions aside from the size/tolerance/location callout for the D-shaped features.
My backgroud with inventor includes less than a year of schooling, learning how to do nothing similar to this. Remodeling this is not hardly a practical option for me with my current level of skill.
Well then,
working with what you have -
Run the Stitch command and window select all the surfaces. (did this not work in 2010)
Delete Face the lofted face(s).
Patch and select the inside loop and set to Tangent.
Select the outside loop.
Stitch it up again.
After patching I get some crazy surface that makes no sense to me.
This is only after adding a fillet. Without the fillet I was getting an error.
@jeregonn wrote:After patching I get some crazy surface that makes no sense to me.
This is only after adding a fillet. Without the fillet I was getting an error.
Attach your file here - your screen capture doesn't look correct.
I still see the Loft and don't understand where or why you are adding a fillet.
What face(s) did you Delete Face? (I will see that when you attach your latest attempt here)
I think maybe you have moved on to another face, but not sure from image.
I am only dealing with replacing the flawed Lofted faces at this point.
Find the red End of Part marker in the browser.
(End of Folded on sheet metal parts EOF)
Drag the red EOP to the top of the browser hiding all features.
Save the file with the EOP in a rolled up state.
Right click on the file name and select Send to Compressed (zipped) Folder.
Attach the resulting *.zip file here.
I suspect you may have missed the second step in JD's previous post:
Looking at the screenshot, you appear to have attempted to stitch the lofted surface into the model.
Try this video - see if it helps.
I had indeed moved onto another face. I was working on smoothing out the transition displayed below.
I now have corrected the surface you were referring to.
Did you set the Patch to be Tangent to the Fillets?
As you move on - attach your file here for additional suggestions.
I did not have any fillets around that feature.
Here is what I am working on now.
Trying to get this to be a smoother transition so when I press my part it will not be deformed here.
@jeregonn wrote:I did not have any fillets around that feature.
Oh you sure do. I am not referring to any fillets you add, I am referring to the existing fillets.
The Patch surface should be set Tangent to the existing, original fillets. This will make the transition smooth between the Patch and the existing geometry. You can set the tangency by editing the Patch feature and selecting the one of two loops in the dialog box that is the inner loop - you will see a setting to the right in the dialog box to set Tangent.
JD is doing a better job than me keeping track of where you are up to on this model!
From your screenshot of the IDW and the previous screenshot with the big red arrow on the IPT, I think you are trying create a convex fillet (as sketched in red on the IDW). Am I right?
If so, this method of creating the fillet might help: http://www.screencast.com/t/bvHjwIaHL
(I created a second fillet just to remove that sharp edge.)
If you are looking for a nice blended shape - apply both fillets, then use "Delete Face" to delete the fillet faces. This will leave you a tidy gap that you can Boundary Patch with tangential edges (as you did previously).
And if I missed the point completely - sorry!
I am pretty sure that I followed those steps correctly, but I am still having the same issue. I need to make it tangent with the opposite sides of the radii. If there is no way I can accomplish this I can just sand it out after its printed but if there is another way I'd rather just get the model right.
I have also attached a copy of my current model, if it does not open let me know and I will try to repost it.
I ended up creating a 3D sketch, usining that to loft and from there I was able to acomplish it.
Thank you both for your help. Would have taken me a LONG time to figure this out on my own.