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Loft problem.
geoff_josey
Member Posts: 65 ✭✭
https://cad.onshape.com/documents/5f44952e7f8d9b30294acab7/w/e13ffc5978e2ad6b37b8a799/e/f2ef8bf8b24e05b0fce401cd
I have been trying to progress a fin design for some while without success even after watching the loft related videos etc.
I am trying use the loft function to create a solid between the 2 aerofoil sections which were imported dxf files. One is on the top plane and the second on plane 1
I have a number of error messages. The most common one is that the direction is not known.
Any help appreciated
I have been trying to progress a fin design for some while without success even after watching the loft related videos etc.
I am trying use the loft function to create a solid between the 2 aerofoil sections which were imported dxf files. One is on the top plane and the second on plane 1
I have a number of error messages. The most common one is that the direction is not known.
Any help appreciated
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romeograham
Member, csevp Posts: 657 PRO
Hi @geoff_josey
You need to select both faces of the each profile as 1 selection, so that Onshape knows that both faces are to be treated as one profile for the loft:
When you select your first face, click the drop-down arrow next to "Face of Sketch 1" and it will now be ready to accept several inputs that it will collect as your first profile.
This "collector" feature works for many feature selection boxes - you can select multiple edges for loft, sweep, etc.
Make sure you click inside the "Faces and sketch regions" box to make it blue, so that you add to your selection for Profile 1, rather than start your selection for Profile 2:
Hope this helps!
Romeo5
Answers
You need to select both faces of the each profile as 1 selection, so that Onshape knows that both faces are to be treated as one profile for the loft:
When you select your first face, click the drop-down arrow next to "Face of Sketch 1" and it will now be ready to accept several inputs that it will collect as your first profile.
This "collector" feature works for many feature selection boxes - you can select multiple edges for loft, sweep, etc.
Make sure you click inside the "Faces and sketch regions" box to make it blue, so that you add to your selection for Profile 1, rather than start your selection for Profile 2:
Hope this helps!
Romeo
Your prototyping supplier may not be able to guarantee that the part that is less than 0.8mm thick will build properly.
You could cut off the part where it is greater than 0.8mm thick, and resubmit.
Moving to the next stage. I now want to put a 12 mm dia.hole vertically thro located 144 mm back from the LE at the top. I put the hole on sketch 1 (top face) and planned to extrude it. The introduction of the circle causes an error in the loft. Is my approach wrong ?
https://cad.onshape.com/documents/335b2ddbd47dcaca7a7d8193/w/9a589dc4e8c59e451f3e8886/e/f2fd44aae491c908c5ad534f
With much appreciated assistance from forum members I completed an earlier model involving lofting between 2 aero foil profiles.
On my current model (see link) I am following a similar procedure ie. importing 2 aero foil sections and then lofting between them.
The aero foil sections are dxf. files with a fairly high number of points defining the profiles.
I now get error messages related to the vertices. i have watched the loft video but cannot related my problem to the vertices issues explained.
Thanks
https://cad.onshape.com/documents/dde1e90dd0eea8d59765c1d3/w/f3fb7245ef0750a25f948be7/e/0d0b2f03ba5e870f01842482
I have sorted it ! The problem was extra centre lines on the 2 sketches.
Also, you may have noticed that you needed to select the face of the sketches, rather than any of the lines that make the edges of the sketch.
Nice!
Thanks for you comment. My lofting success rate is still erratic !
Please clarify your "select faces" comment related to the rudder model.
https://cad.onshape.com/documents/9829afe78e3722bf4b962bab/w/812a932c6d493b307c6b537d/e/a0989b1df5fc9e819ce7d578
I am trying to loft between the 2 outline aerofoils which were imported as dxf files.
On this example is the face you refer to the plane ?
I think my problem is in the selection procedure.
In Onshape, when a sketch has elements that enclose a region (it can be with overlapping lines, or lines that meet at vertices), the region becomes shaded, and selectable.
Here's your sketch with some lines removed so it doesn't create a closed region:
Here's the shaded region (showing that the sketch encloses a region:
For a Solid Loft, Onshape can use the face of the profiles as inputs - so you can just click the shaded region that is enclosed by your sketch elements.
Another area where you may run into issues when getting started with Onshape is the selection of profiles. If you want to "collect" several selected elements together to be one profile, you can do so, if you use the little drop down arrow in the selection box:
You can see the 3 edges selected in the first Profile will be connected together as one profile.
For a surface loft, you need to select edges (of a sketch or body) and for Solid Loft you need to select faces (of sketches or bodies).
Hope that helps!
I have tried this loft as a solid and a surface without success,
I am trying to understand the message " loft did not generate properly Point profiles can only exist as first and last profiles.
Any help appreciated Thanks
https://cad.onshape.com/documents/b6f8b2b6ff334ae88bddd6ef/w/15ac58617d56a7e1068c92de/e/66468554fcf448e6d533f74b
Sketch 1 and Sketch 2 have multiple sets of lines in them. Somehow, the DXFs have duplicate data sets so that when you import them into the Sketch 1, you get two sets of lines "on top" of each other. This is likely causing you selection issues, so that your features don't complete properly.
Even though there are extra lines in the sketches, you can still select the face of the sketch and a solid loft completes.
With the extra lines in these sketches, I would NOT recommend trying to make a Surface Loft (because a surface loft requires edges as inputs).
To delete the extra set of lines, you can select each line segment individually, and press the delete key on your keyboard. The sketch will look the same, because there's another line below it (you can't use box-select techniques, because it will select both lines). This will be a lot of work.
However, you don't need to deal with the lines at all. Some of the lines are creating an enclosed region, which means you can select that to do your loft.
To make this easier, I used the Offset Surface tool (with 0 offset) to create a surface body (by selecting the face of the sketch). Then you can select that surface face for your loft.
Create some Guide curves. Use the Bridge Curve to do this.
Then you can make your selections for a Solid Loft, and use Guide Curves:
The loft will complete, and won't be twisted.
There are many, many faces in this loft - and you may have performance issues or difficulty with subsequent features. There are other discussions on the forum about creating a single spline form airfoil data that will likely help.
Good luck!
I was using an obsolete level of the software. When I used the correct level only a single outline was generated. I would have never found this one without your help ! The loft now looks good but I now need to add some more features
I am now trying to repeat the process with different aero foils and dimensions. I have read all the forum replies again and watched the loft videos to refresh my memory. I have checked duplicate profiles etc.
I can extrude both the aero foils, but a loft fails and gives the message "Loft 1 did not generate properly. Point profiles can only exist as first or last profiles"
To check for me making basic errors I created a very simple model and to my surprise this gives the same error message. I think I must be missing something !
https://cad.onshape.com/documents/9eecb066fea59b1c612e527e/w/8490588c82a436fd36a280dd/e/053e9c5fe77dd39c0cf36bc5
Would you save the failed loft you are getting so that it can be analyzed? I was able to create a loft as a solid or surface based on your profiles without any trouble.
https://cad.onshape.com/documents/9eecb066fea59b1c612e527e/w/8490588c82a436fd36a280dd/e/053e9c5fe77dd39c0cf36bc5
You have bad sketch geometry in the top sketch.
https://cad.onshape.com/documents/c34bd5bc06c2f2822c85ba3a/w/31d4c45002fdb5d5edaa0741/e/1eeed4513c9b6ca78c42fbbe
You have way too many things selected in your loft feature dialogue (the tool is confused as to what you want to loft from and to) you should only have 2 selections in this application. Select only the face of each sketch or if you need to select the edges for some reason then research how to add a segment to the already selected segment within the loft dialogue.
I understand the note ref. only selecting eg. the 4 edges, but I do not see the edges as an option. I would have thought the default would be no selections allowing me to select what I want. I seem to get everything selected as the default.
https://cad.onshape.com/documents/c34bd5bc06c2f2822c85ba3a/w/31d4c45002fdb5d5edaa0741/e/1eeed4513c9b6ca78c42fbbe
Take a look at this document I did the loft 2 different ways. Loft 1 was done by selecting the face of the sketchs. Loft 2 was done by selecting edges.
https://cad.onshape.com/documents/17510f1747441878eb396274/w/4e18a7d3c445df6afa104534/e/4238085e8d0af709c9aebd9e