Hello,
I'm currently trying to smoothly cut a sketch out of a part I created. In the picture below I made a cut extrude which results in sharp edges. This is not what I need. Sadly my surface is not even so a sweep cut doesn't work.
I already tried some other techniques, but none resulted in a smooth shape. The smoothness is essential since it's needed for aerodynamic reasons.
Do you have any suggestion how I could accomplish this?
Thanks in advance.
Can you attach the part? I am not clear on what you want the cut to look like. Can you just add fillets to the sharp edges?
Fillets create horrible errors - maybe I use it wrong but it was impossible for me to make it. Here's the part.
I am getting an error when I try to open the file. Maybe there was a problem with the file uplaoad. Can you try attaching it again?
You could try cutting with a sweep. Create a sketch of the profile you want, and sweep it along a 3d sketch path along the trailing edge.
Don't know what happened. Try to reupload:
Yeah I tried that already and I had no success. Could you point it out step-by-step for me? I guess I made a mistake somewhere.
I tried downloading as well, but I also get an error. What version of SolidWorks are you using?
It still won't open for me, and i don't know why. But from your image my best advice would be to modify the shape by editing the loft profiles. For example edit every other profile, trim the front off of it, and add a shorter curve. If the profiles aren't located exactly where you want the ridges then you might need to add more profiles.
Yes that's exactly what I need. How did you modify the loft profiles? I use curves converted from an airfoil and this seems a bit tricky to me.
Since the file's not working for you I'll post a snippet of my sw window. How do I transform the curves that they look like the ones you did?
I'm using the latest version of Solidworks (2015).
You have a couple options here, but here's what I think might be easiest. First roll back to just after the loft but before you create the hub. Create new planes across the blade at each high and low spot of the curve you want. Then on each plane start a sketch and make an intersection curve using the solid body. This will trace the original blade profile into the sketch. For each sketch that is for a low spot on the curve, trim the intersection curve back to where you want the profile to start deviating. You can do this by sketching a line across it and then trimming the front portion of the curve.
Next sketch the new front profile you want for the blade. You could use an ellipse portion or a spline or whatever you want. Just make the new front curve tangent continuous with the back part.
If you already have a sketch for the wavy front end you could make a point on the spline and make a pierce relation with the wave, or if the wave sketch is on a 2D plane offset some distance from the actual prop then you could draw a vertical construction line with one end pierced by the wave and the other end on the front of your sketch.
So eventually you should have a bunch of sketches alternating between the original profile and a modified profile. Now you can make a new loft using your sketches instead of the original curves, and then delete or hide the original loft body. To get the new loft to work you might need to show the connectors and adjust them to follow a smooth path.
Let me know if any of that was unclear. Or if you want you could save the blade (just up to right after the loft) as a parasolid and then upload it. I could try out this method on that.
Okay so first of, I tried to convert the curves in a sketch. I made it as you suggested with a plane and an interselection curve. Then I added the line. Now I normally should trim the sketch to the line, but this doesn't work. It trims always the line, but not my sketch. What I do wrong?
Its hard to say why the trim isn't working correctly. You are in a 2D sketch, right? Maybe you are using the trim tool wrong. And you have Power Trim (or in your language Intelligentes Trimmen) selected, so you just need to click and drag across the part of the sketch you want to remove. Like drag where I have drawn the red line below. Then it should remove the curve and not the line.
Okay maybe this is more helpful: Once I try to drag I shortly get a little tooltip saying "A closed element cannot be trimmed or extended"(my own translation). Is my spline maybe somehow protected?
Start the click drag off of the line, and drag over it (like my red line). BTW the English message you mentioned is "Cannot use a closed entity for trimming or extending", so your translation was pretty close!
Ugh, can't drag anything except the straight line itself. May I can send you the complete file with folder? (Since there was a opening issue last time)
extrude a separate part or surface on a flat plane in right place then select "tools-sketch tools-intersection curve. Select meeting curve of 2 parts. you can then hide or delete that part or surface
I just saw that you are using SW2015, so that is probably why I can't open the file (I am on 2014). It is strange that it didn't say Future Version. I'm still not sure you understood my trimming instructions though. You shouldn't try to click on and drag the curved line, you need to click out in open space and drag across the line, then it will trim the curve back to the straight line. The other thing you can do is use "Trim to closest" (or in your version "Zu nachstem Element trimmen") and then try clicking on the part of the curved line you want to remove.
Yes, that worked! Took some time, but now it's fine after all. Thanks! So one thing's left: How can I trim the spline each time at the same place? I mean, I don't want to cut the spline just based on my estimation, but always at something like 3mm(front -> line to cut).
Thanks for your answer, but I think you overestimate my capabilities you mean I should duplicate the part?
That's a good question. You could get it close by sketching a point on the front tip of the profile and then dimension the trim line from that point. But I don't actually know how you could constrain the point to the exact tip. You might need to just position it close by eye and fix it.
So, I now made all the trimming and well I tried to create the loft, but once I included more than the sketches you see in the picture below the loft throws me the error that it can't be build. (The geometry is cutting itslef/self intersection - free translation). Any idea why this happens? I only altered the curves as you instructed me and added a tangential curve on the trimmed area.
EDIT: Got it, had to combine all the curves. Now there are two things left to success Which kind of curves could I use that gives me a more eliptical shape in comparision to the tangetial curve? And how can I dissolve the relation between the old loft and the sketches?
For the leading edge curve you could use an ellipse segment rather than an arc. There's a tool to draw an ellipse segment but it is kind of tricky getting the portion os the ellipse you want, so I think it's easier to draw a complete ellipse, position it, and then trim away what you don't want.
For your other question, I wouldn't try to modify the original loft. I would just hide or delete that body and then make a new loft using your sketches.
Okay that's a good point, I'll try that. The problem with the loft is that the skecthes are dependant on the original loft and so are the cut extrudes that I have to create my socket. Can I some how move the dependencies from the original loft to the new loft?
The best answer I can give is that it would be better to learn how to produce smooth surfaces from the start.
Hope I do not sound too critical but this is certainly the best solution.
You have a couple options here, but here's what I think might be easiest. First roll back to just after the loft but before you create the hub. Create new planes across the blade at each high and low spot of the curve you want. Then on each plane start a sketch and make an intersection curve using the solid body. This will trace the original blade profile into the sketch. For each sketch that is for a low spot on the curve, trim the intersection curve back to where you want the profile to start deviating. You can do this by sketching a line across it and then trimming the front portion of the curve.
Next sketch the new front profile you want for the blade. You could use an ellipse portion or a spline or whatever you want. Just make the new front curve tangent continuous with the back part.
If you already have a sketch for the wavy front end you could make a point on the spline and make a pierce relation with the wave, or if the wave sketch is on a 2D plane offset some distance from the actual prop then you could draw a vertical construction line with one end pierced by the wave and the other end on the front of your sketch.
So eventually you should have a bunch of sketches alternating between the original profile and a modified profile. Now you can make a new loft using your sketches instead of the original curves, and then delete or hide the original loft body. To get the new loft to work you might need to show the connectors and adjust them to follow a smooth path.
Let me know if any of that was unclear. Or if you want you could save the blade (just up to right after the loft) as a parasolid and then upload it. I could try out this method on that.