Need help with Alibre

Home Model Engine Machinist Forum

Help Support Home Model Engine Machinist Forum:

This site may earn a commission from merchant affiliate links, including eBay, Amazon, and others.


Model Engineer
Project of the Month Winner
HMEM Supporting Member
Nov 19, 2008
Reaction score
Sterling Heights, MI
Do any of you alibre users have any tips, tricks, or wisdom concerning lofts with guide paths? i am truing to draw the fenders for the little shriner car so I can 3D print them. Because I couldn't find a way to get an existing STL into Alibre I was forced to try and draw it from scratch. I didn't even know what the loft feature did until 3 days ago.

I have 2 side panels that lofted from one sketch to the other with no trouble. When I add the guide path to the mix I get this error.

ACISERROR_SKIN_GUIDE_NOT_INTERSECT: The guide curve does not intersect all profiles.

I have tried different paths, moved the plane, watched video on youtube, it just doesn't want to work on these 2 panels. I just need them to loft up to fill in to the top of the fender and i will be done! The guide paths have worked well in other areas of the model.

In the picture you can see the guide path sketch. It is the same radius as the fender and perfectly aligned. Anybody skilled in the loft command I could use some guidence here.

Should not be a problem opening an STL, Just double click it to open from file manager and it will ask you what to open it with, go down the list of programs on your computer and select alibre.

I'll send a PM
Hi Steve
I use Solid Edge. If you send me the STL I can open it and save it in a format you can open.
It will just be a dumb blob. At least for me it is. It comes in at original size, but I cannot select anything. I can sketch over it in MY "planes" And it will cut just fine so it can be edited. just kind of crudely.
If you would like to try it, PM me and I'll send you me email.

Can you open the stl in fusion 360 (or have someone else do it) and export in Step - then open that in Alibre?
I had someone try that in solid works. They imported the file and saved in solid works. I could not open it. Trying to convert has been a huge failure. I also cannot send the stl file. It's 96meg and my email program doesn't like it.
you can use the service for free to send large files. Solidworks files can be read by Alibre. Not certain about 3-year-old software but I was converting Solidworks files back then. I do have the top end of the Alibre software and that might make a difference. If you are a veteran, you can get the entire repertoire of Solidworks including the CAM for $20 a year.
I took a look at your car project thread and the model makes sense now.
I'm not quite sure if the blank section is all that's left or if the blue selection is part of what you are trying to fill. If you are only trying to fill the left over gap then the loft feature will not work.

This might be the plan I'd take.

Lofting a test in Alibre was a learning experience for me, as I haven't really messed with it yet. It is very sensitive to datum plane normals and curve polarity flipping, and there are no obvious controls in 3D space to adjust them on the fly. Even how I drew the sketch rectangle [bottom left to top right or vice/versa] for the orange below changed how it calculated the loft. Reversing the plane polarity that it was sketched on also affected the solution.

Still needed one more variable to flip but bed time. Alibre does not provide a means to correct normals or profile matching that I know of yet. Bottom line is yours is going to require a unique solution. Even if we can't save, the pipeline used to get it to work might help.

Another option is to block out the shape, fillet it, and shell it. You can then avoid the lofting challenges and future edits might be more stable.
sorry, mixed it up with STP file.

I should be able to convert an STL into a solid in F360(done it a couple of times) and then export it as a STEP which can then be opened in Alibre

See the message I sent earlier.

I also had a go at the loft in F360 which often copes with curves better and by deleting your "blue" loft and drawing a long narrow rectangle on the top of the running board I was able to loft that rectangle to the curved underside of the downturned fender. This looks OK as the panel starts off flat and then takes on a gentle curve so it meets the fender correctly.
Steves fender.JPG
Last edited:
Hello Jason! That's what I need right there. Can you export that file to STP and send it! I am very interested to see how you made it work.

I don't have the stl files anymore. The person that donated them had them on an online drive and is no longer available to me. My only hope is to draw them myself.
I'll add th erear one this evening and send it through to you.

Can you just let me know the length of say the running board so I can make sure I've not converted it from inch to metric as a 1/25th scale model may be smaller than you were thinking of!
Not quite perfect but as close as I think I can get it. Use the second file I sent you Steve
Steves fender lofted.JPG
I also found a fix for the problem.

Instead of trying to loft between 2 sketches with a guide curve I added more sketches and lofted over 3 sketches on the rear and 5 on the front. The curve under the fender is produced buy the geometry between the 3 sketches. I dont know why but it worked like a charm. Just took me 4 days to figure it out. Before sunday I had never heard of lofting. Its a nifty tool in the program but im guessing it would take a long time and frequent use to really get it figured out.

Thank you to Jason B, Gary D and anybody else who offered help!!


Just to throw it out there, when i have gotten that error with the lofting tool, it is because the guide curve is not connected to sketches at both ends. I love the tool but it is a picky PITA. The end of the guide curve HAS to be be connected to 2d sketch on both ends. I have found that the 3d tool will not happily connect to what you want. Usually i will add a node where the lines are for my sketch then use those as my start and end points.
  • Like
Reactions: Zeb
If you send me the STL I can open it and save it in a format you can open.
It will just be a dumb blob. At least for me it is. It comes in at original size, but I cannot select anything.

Right. An STL file contains only a set of x,y,z coordinates that define triangles; the triangles approximate the surface of an object. No underlying geometry that might have been used to create the object is included, and in fact, no units. Technically, the coordinates used to define the triangles are considered to be arbitrary units; most people treat them as millimeters, and most software defaults to creating the STL in such a way that the size comes out right if you treat them as millimeters, but technically they could be considered anything you want - inches, meters, miles, lightyears ...

Another option is to block out the shape, fillet it, and shell it. You can then avoid the lofting challenges and future edits might be more stable.

I was thinking the same thing! I am interested to see that lofting is not an easy or error-proof process in Alibre; my only 3d CAD experience is with FreeCAD, in which lofting sometimes works brilliantly ... and sometimes not. I have learned that it can often be vastly easier to do as Zeb suggests, making a solid that is then shelled and trimmed - at least, this is the case in FreeCAD, and it seems perhaps also in Alibre. Perhaps also true for Fusion360, or SolidWorks, or others??
I think all solutions can be legitimate. It really comes down to what you're used to a year down the road. Most people can remember how to block, cut, and fillet. Tangency may be a little off trying to close that geometry using a loft, but it can always be sanded out on the print or plug tooling.
The other two solutions I might try as a last resort but maybe not recommend here are:
  • Surfacing in Rhino/SW
  • Import accurately proportioned guide curves to Blender and model with subdivision surfacing.
Something on the design side. You could add some meat to the attach points on the step and add a rib on the bottom surfaces above each axle so the loads dump gradually from the wiggly bits.
I think I would try the "Shell" approach or sweeping an extruded profile (a "Thin" extrusion that allows me to add thickness to my sketch) along a curve that would be the outside profile of the fender (viewed from the side) & then create the side walls/running boards as flat extrudes before I would try lofting or "swept trajectories" (or whatever your software might call it), these features often seem (as you have found) unpredictable & difficult to modify in some cases.