Loft problem.

geoff_josey

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

romeograham

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!
Romeo

romeograham

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!
Romeo

geoff_josey

Very helpful. many thanks

geoff_josey

I have now run into another problem. I have modified the model to sweep the profile. All looks good and I thought it was solid as that was specified in the loft. When I issue the model for a quote they say the wall thickness is below 0.8 mm ! Not sure why and how do I check that the model is solid ?

romeograham

The body is probably solid, but the end of the airfoil is less than 0.8mm:


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.

geoff_josey

I have asked the supplier to verify the cause of the problem. Awaiting a reply.
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

NeilCooke

Add the hole afterward rather then trying to include it in the loft (loft doesn't like sketches with internal profiles)

geoff_josey

That is what I tried to do. I have completed the loft and it looks good. I then added a test hole on sketch 1 (top) and tried to extrude with the remove option. I then get extrude and loft errors.

NeilCooke

But you edited Sketch 1 which will affect the loft - create a brand new sketch for the hole.

geoff_josey

Got it - thanks

geoff_josey

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

geoff_josey

I have sorted it ! The problem was extra centre lines on the 2 sketches.

romeograham

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!

geoff_josey

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.

romeograham

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!

geoff_josey

https://cad.onshape.com/documents/9dda3d78b8184e390d736254/w/2093736061057e01cbc0257b/e/6c4e22606b5b37b78ebe60a8
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

romeograham

@geoff_josey There are some issues that are making this more difficult than it needs to be. 
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.

Make sure you select points that prevent twisting. I used the points next to the Front Plane:

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!

geoff_josey

Many thanks for your help and the great detail. I have been back into the software that created the aerofoil sections and spoken to the originator.
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

geoff_josey

With help, earlier, I managed to create a loft between the 2 aero foil sections and had a 3D printed part made successfully.
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

geoff_josey

I am not sure if people will read my post as it was a continuation of a post on Nov 6th  marked "answered"

glen_dewsbury

geoff_josey said:

With help, earlier, I managed to create a loft between the 2 aero foil sections and had a 3D printed part made successfully.
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.

geoff_josey

This is the failure for the test one.

https://cad.onshape.com/documents/9eecb066fea59b1c612e527e/w/8490588c82a436fd36a280dd/e/053e9c5fe77dd39c0cf36bc5

wayne_sauder

@geoff_josey
 You have bad sketch geometry in the top sketch. 

glen_dewsbury

There are some mismatches in your sketches that are causing the problem. Over lapping of arcs and lines will not work with the method of lofting chosen. You probably want to add tangency for all lines and arcs for a smooth transition. Make ends of lines and arcs coincident. See last sketch added to the sequence below. There is a lot of extra selections in tour loft feature. With sketch corrections you will be able to make a surface or solid by selecting the shaded face of the sketches. A surface could also be generated by multiselect of edges if you choose. Only needed if match connections needed (not with these profiles).

martin_kopplow

I have modeled some aircraft and other airfoiled things in the past. One thing I learned was that all the downstream trouble I got into by importing DXF airfoils (From Xfoil, airfoil databases, or whatever) and directly modeling on them does not save any time compared to first building a clean spline based sketch on them. Those DXF files usually have limited accuracy, and my former CAD system fortunately had a tool to import spline coordinates as a text file, then approximate curvature steady splines on them. Does such a tool exist in Onshape? If yes: Where? If not: I'd appreciate it.

geoff_josey

Thanks for the help. I have now created (hopefully) 2 simple outlines on 2 planes without the errors that have been pointed out. I can again extrude both profiles, but a loft attempt fails with the same error message as previously.
https://cad.onshape.com/documents/c34bd5bc06c2f2822c85ba3a/w/31d4c45002fdb5d5edaa0741/e/1eeed4513c9b6ca78c42fbbe

wayne_sauder

@geoff_josey
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. 

wayne_sauder

Example of edge selection. 

geoff_josey

Still confused ! The only way I can achieve the loft is to extrude both profiles as per the link. I can then select the 2 faces and complete the loft. Can you make the face selection from just a profile ?
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

wayne_sauder

@geoff_josey
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

wayne_sauder

Both methods yield identical results. Turn the surfaces on or off to compare.