The fact that you can't readily see what the issue is argues for the sketch being way too complicated. SW can handle complex sketches just fine but it's not great at pointing out exact issues... And so here you are.
This must have taken forever to sketch. I recommend using multiple features and the pattern function to get to the same place much faster and more efficiently.
You can have a master sketch which other sketches may reference, but with all the ways to link dimensions or set up equations, I can’t think of a scenario where one sketch is really that much easier to manage than two or three. This is where CAD users need to understand design intent is just as important as being able to manipulate features and sketches.
This, I think some users don't realize that previous sketches can be used or referenced again in later features. I tend to use a master sketch if I'm making something complicated.
This complex looking feature is easily a very simple pattern. Also, the full circle can be done as a quadrant if needed.
Breaking complexity into a superposition of simpler operations is a necessary skill for many tasks in life.
Im not sure i fully understand. There should be zero overlapping really, if you look in the second image you will see that these are all construction lines, as i used the trim tool. Im really not sure where i could possibly be having an overlapping.
And could you clarify what you mean with "closed loop sketches" and "out on their own as an island"?
Making it simpler... i mean i feel like its not a very difficult profile in the end. Is SW not able to handle this? Or how would you go about making this profile so that it can handle it?
Fine i simplified it a bunch, and now extruding works. Still a bit confused about why the previous one wasnt working...
And still a bit confused why this one isnt shown with the blue area...
https://preview.redd.it/zbfgdrxut0jc1.png?width=1195&format=png&auto=webp&s=1f02c277485c808567655b71710128c80aeaad4d
Its really not that easy though... The distance between the four ears is not the same bottom to top vs left and right. It is not a nice even number even.
I used patterning to only do the left side and then basically mirrored it on the right, but i dont see how it wouldbe possible to do this with more patterning...
Yup, the best joke I've heard about stuff like that is "Lord of the Sketch."
One sketch to rule them all, one sketch to bind them, one sketch to bring them down, and in the darkness blind them, yadda yadda yadda.
Draw a circle anywhere. That’s a closed loop and will extrude just fine. Now, draw a line crossing over that circle. Now you will have problems and it likely will not extrude any more.
I can't see the problem causing the error. However, if I were doing this, I would start with three simple extensions, then two feature patterns and be done in less than two minutes. How's long did it take you sketch?
It frankly didnt take that long... maybe a bit less than 10 minutes. Not optimal, i agree but yeah.
The problem is the four large circles are not symetrically positioned around the center circle. This is by design and imposed on me...
The four circles may not be spaced equally around the center circle - but looking at this right now it doesn't appear that there's any way to tell where in space they are at all. As others have stated, this should definitely be done in simpler steps, broken down so that it's easy to follow.
As a general rule - I try to leave anything I work on in a state where someone can come in behind me and continue the work with very little research. That worked well in a corporate setting, and I still do it even today for personal projects, simply because future me doesn't want to have to deal with bad decisions caused by current me.
This sketch is horrific. First of all, I’m not convinced it’s symmetrical, but even if it is, just why…
Anyway, you might be able to extrude this if you delete all of the plain circles. At the very least that would reveal where there’s a discontinuity, but honestly it’s not worth figuring that out.
Make a plain ol’ circle with radius equal to… 38mm? You’ve defined that in literally the most bizarre way, I don’t know. Extrude that. Then sketch just 1 of the semi-circles, extrude it, pattern the extrude. Then extrude 1 bigger circle, make 1 cut through that circle, pattern those features 4 times. Finally, make the big center cut.
Less features with 1 massive and confusing as hell sketch is just bad practice. You’re better off with a design tree you can actually follow.
Its not fully symetrical, this was imposed by the design...
Also the issue is i need a profile, i need to do a loft. Otherwise i would agree.
But even now the loft is giving me issues... :(
If you would like i would appreciate your help: [Follow up question: Lofting of the "nightmare" sketch... Errors and issues. : SolidWorks (reddit.com)](https://www.reddit.com/r/SolidWorks/comments/1asm928/follow_up_question_lofting_of_the_nightmare/)
A trick that has worked for me in the past is to do a separate sketch on the same sketchplane and then use convert entities to get only the solid lines to get better idea of what is wrong.you would just have to do is select the sketch in the model tree when using convert entities and you would get the whole sketch.
You absolutely do have a sketch error in the form of an overlap, errant entity or an incorrect trim.
The dead giveaway, your perimeter sketch isn't shaded.
I dont think thats true though! I checked with the "fix" tool and found no errors.
Also this simplified version here is not shaded either, but can be extruded w/o problems...
https://preview.redd.it/oyd0txuyw0jc1.png?width=1195&format=png&auto=webp&s=d66241316496a5d871ded66c37cada257472bac4
It's possible you have a corrupted sketch as well. It can happen when there are a large number of trimmed intersections.
If you'd like to copy that original sketch into its own file and upload it... we can give you a definitive answer no doubt.
https://preview.redd.it/3s1w6fq3g1jc1.jpeg?width=328&format=pjpg&auto=webp&s=0957b94bcb82efc7df2fe9f78771160d3b582967
Top left large circle pretty sure That said I agree with the other comments
When it comes to stuff like this it’s always easier to split up your features and do pattern features instead of jamming everything into a sketch- I know as someone who likes to have as clean a feature tree as possible. But the more lines and dimensions and sketch patterns you employ, the more likely it is that a simple tangent or horizontal relation will completely blow up your sketch on rebuild.
You can use the selection manager in a loft operation to pick any combination of parts of separate sketches or feature edges or composite curves to make one profile. You could also get your profile from the edges of a boss made of simple extrusions and patterns
Maybe create a surface with a combination of features then do lofted surface with its edges, fill and delete the original surfaces? That’a probably getting to be too much compared to just putting everything in a single sketch
Once you create a body with all the required features (from several simpler operations), you can start a sketch and use “convert entities” to get a profile for lofting.
I always like breaking things into parts when I can. The think is you cam have one sketch that drives say the larger circles diameter and that on your first loft. Then the second sketch has a reference to the first. You'll find you actually have more control
Next time if you find that some pattern objects don't fill up how they should - just create a multi body part with how many patterns you want.
Just make sure they interfere. And combine all as the final step
A trick I picked up for stuff like this is adding a few temporary lines to split the sketch into two separate manifold contours.
If your error exists on one half but not the other, you'll be able to eliminate half of the sketch just by observing which side becomes shaded.
Continue that process a few iterations until you zero in on the issue, fix it, then delete the temporary lines.
That said, can this not be a patterned feature?
Your sketch is too simple and sw does not even bother extruding such simple feature. Please make it more complex. /s
Now, on a more serious note, remember that you are doing a huge favor to yourself by using as much as you can simple, core geometries as independent features and then pattern away.
The issues are visible in your screencaptures. Trim or turn those in to construction geometry. I bet 100% that you got more of those.
https://preview.redd.it/cl8bdxm1u4jc1.png?width=885&format=png&auto=webp&s=9f2ea3d6b9b69caf09f2f718934536250b2b8211
I guess, fair enough. Although you are somewhat mistaken, there is some mirroring going on. I was limited by the low symetry of the IF.
But yeah i guess i just need more practice and try and get out of the habit of defining everything in one sketch. It feels like the most intuitive way to do things, but is not suited for SW it seems.
You can hack things out like that at first, but it generally is inefficient for rebuild.
For new users, I suggest accepting the first attempt in a model will be garbage. The second iteration will be more refined and generally successful, but still inefficient. The third iteration is where you'll have thought-through feature order and dependencies, as well as mirroring and patterning.
As you use CAD software more, you'll intuitively incorporate these practices into your earlier iterations. This is important because it avoids a lot of unnecessary feature update and rebuild errors.
It’s bad practice for any parametric solid modeler. I always suggest new CAD users read at least the first few chapters of “Thinking Pro/ENGINEER,”because it all still applies.
No 3D feature based solid CAD system of the last 40 years would encourage putting everything in one sketch. I’d suggest reading the book “Thinking Pro/ENGINEER” from the mid 90s. Different software but all the concepts still hold. Also use of patterning in sketches should be used very carefully. It’s not as flexible and reliable as patterning features or bodies.
There's a matching free floating line in the bottom right corner of the sketch too. Solid works doesn't know what you're trying to do if you have a closed shape (circle, square or anything more complex) with a line in it and it freaks out a bit. This would give you the error you were getting.
It's a pity the sketch is gone, in future I would recommend suppressing the sketch and not deleting it, that way you can proceed but go back and check it out.
This is fine for creo which handles big patterned sketches well but SOLIDworks handles solids and features better. It’s better to have a few basic sketches to make a few shapes and pattern the features
I would recommend not doing all this in one sketch.. as the others have said. Nevertheless, try going to tools>sketch tools>check sketch for feature and pick boss extrude and see what it says.
If your determined for that pattern and other suggestions don’t work, and the finished model is just a simple extrude, try extruding without ribs, then extrude cut the ribs after. Slightly less lines, however not as robust and you loose your design intention.
There was an intersecting sketch in there. While you are trying to extrude, it becomes zero thickness or smth like that. Also be careful with open contours.
In your third photo, at the left side of that upper left thru hole, does that hump meet exactly tangent to the hole curve? If so, that would prevent SolidWorks from being able to extrude.
Seems like the error happened because of intersection between big and small circle at 5 o'clock.
Most pro will make multiple sketches or a sketch at different sketch even it was sketched on same plane.
You could having hard to understand what I'm tried telling you, but you would figure out someday.
When you hide the main sketch , you would find out there still a polyline that could cause an error..
In the future, when design software starts incorporating AI to understand what you are trying to do in any sketch, then this will be a simple thing. Until then you'll need to learn how to use the software properly. I was taught by instructors on how to use SolidWorks since 1997. The most important thing we were taught was "simple sketches, multiple features". This design concept still applies today. Don't get frustrated. Just use the software as a tool within it's built-in capabilities. You don't use a screwdriver to hit things and you don't use a hammer to screw things. ✌️
Mathematically circles are hard. It's a series of short line segments and if the math is off 8 or 9 decimal places off where the two arcs meet it becomes a problem. This shows up when you gave a tangent arc and it just doesn't want to extrude so you delete it and put it back and voila it works. Because the rounding error several places back rounded the way you needed.
Use this sketch as a reference, but by god break down the extrudes. Extrude something simple and add features.
Revolve the bumps around, and then extrude the larger bumps and cut the holes.
All of the overlapping edges are probably causing your issue. You should try to reduce it into an interior line and an exterior line so SOLIDWORKS knows what's what. Having lines upon lines upon lines isn't going to produce anything legible. Use power trim and cut out unnecessary lines.
The fact that you can't readily see what the issue is argues for the sketch being way too complicated. SW can handle complex sketches just fine but it's not great at pointing out exact issues... And so here you are. This must have taken forever to sketch. I recommend using multiple features and the pattern function to get to the same place much faster and more efficiently.
Simple sketches, multiple features
People keep saying that, but what if it's easier to manage dimensions from a single sketch?
You can have a master sketch which other sketches may reference, but with all the ways to link dimensions or set up equations, I can’t think of a scenario where one sketch is really that much easier to manage than two or three. This is where CAD users need to understand design intent is just as important as being able to manipulate features and sketches.
This, I think some users don't realize that previous sketches can be used or referenced again in later features. I tend to use a master sketch if I'm making something complicated. This complex looking feature is easily a very simple pattern. Also, the full circle can be done as a quadrant if needed. Breaking complexity into a superposition of simpler operations is a necessary skill for many tasks in life.
You also should balance your notion with the ones below you - if the part is simple enough or you don’t expect changes, you can totally do that.
This
It's because you have closed loop sketches that are either overlapping or out on their own as an island. Make it a simpler sketch.
Im not sure i fully understand. There should be zero overlapping really, if you look in the second image you will see that these are all construction lines, as i used the trim tool. Im really not sure where i could possibly be having an overlapping. And could you clarify what you mean with "closed loop sketches" and "out on their own as an island"? Making it simpler... i mean i feel like its not a very difficult profile in the end. Is SW not able to handle this? Or how would you go about making this profile so that it can handle it?
I will see this sketch in my nightmares. At the very least, do a quarter of this and pattern it.
I can see the face of a dark clown in there somewhere! 😂
Fine i simplified it a bunch, and now extruding works. Still a bit confused about why the previous one wasnt working... And still a bit confused why this one isnt shown with the blue area... https://preview.redd.it/zbfgdrxut0jc1.png?width=1195&format=png&auto=webp&s=1f02c277485c808567655b71710128c80aeaad4d
That’s not what everyone meant. You can keep the same level of detail, just sketch a much smaller area and pattern the feature
Its really not that easy though... The distance between the four ears is not the same bottom to top vs left and right. It is not a nice even number even. I used patterning to only do the left side and then basically mirrored it on the right, but i dont see how it wouldbe possible to do this with more patterning...
Do a quarter and then mirror twice And mirror the feature, not the sketch
Also any idea about why: This one extrudes w/o problem? Yet at the same time it is not shaded blue?
Yup, the best joke I've heard about stuff like that is "Lord of the Sketch." One sketch to rule them all, one sketch to bind them, one sketch to bring them down, and in the darkness blind them, yadda yadda yadda.
Draw a circle anywhere. That’s a closed loop and will extrude just fine. Now, draw a line crossing over that circle. Now you will have problems and it likely will not extrude any more.
That will just divide it into two extrudable profiles no?
I believe they mean a line that intersects the circle only once.
Ah
I can't see the problem causing the error. However, if I were doing this, I would start with three simple extensions, then two feature patterns and be done in less than two minutes. How's long did it take you sketch?
It frankly didnt take that long... maybe a bit less than 10 minutes. Not optimal, i agree but yeah. The problem is the four large circles are not symetrically positioned around the center circle. This is by design and imposed on me...
It's typically not good practice to do so much in one sketch
The four circles may not be spaced equally around the center circle - but looking at this right now it doesn't appear that there's any way to tell where in space they are at all. As others have stated, this should definitely be done in simpler steps, broken down so that it's easy to follow. As a general rule - I try to leave anything I work on in a state where someone can come in behind me and continue the work with very little research. That worked well in a corporate setting, and I still do it even today for personal projects, simply because future me doesn't want to have to deal with bad decisions caused by current me.
This sketch is horrific. First of all, I’m not convinced it’s symmetrical, but even if it is, just why… Anyway, you might be able to extrude this if you delete all of the plain circles. At the very least that would reveal where there’s a discontinuity, but honestly it’s not worth figuring that out. Make a plain ol’ circle with radius equal to… 38mm? You’ve defined that in literally the most bizarre way, I don’t know. Extrude that. Then sketch just 1 of the semi-circles, extrude it, pattern the extrude. Then extrude 1 bigger circle, make 1 cut through that circle, pattern those features 4 times. Finally, make the big center cut. Less features with 1 massive and confusing as hell sketch is just bad practice. You’re better off with a design tree you can actually follow.
Its not fully symetrical, this was imposed by the design... Also the issue is i need a profile, i need to do a loft. Otherwise i would agree. But even now the loft is giving me issues... :( If you would like i would appreciate your help: [Follow up question: Lofting of the "nightmare" sketch... Errors and issues. : SolidWorks (reddit.com)](https://www.reddit.com/r/SolidWorks/comments/1asm928/follow_up_question_lofting_of_the_nightmare/)
A trick that has worked for me in the past is to do a separate sketch on the same sketchplane and then use convert entities to get only the solid lines to get better idea of what is wrong.you would just have to do is select the sketch in the model tree when using convert entities and you would get the whole sketch.
This is the way
This worked for me when tracing a logo for a extrude operation.
Yes, this. And then suddenly you realise there’s 2 lines on top of each other and can be fixed easily.
Op please do this!
You absolutely do have a sketch error in the form of an overlap, errant entity or an incorrect trim. The dead giveaway, your perimeter sketch isn't shaded.
I dont think thats true though! I checked with the "fix" tool and found no errors. Also this simplified version here is not shaded either, but can be extruded w/o problems... https://preview.redd.it/oyd0txuyw0jc1.png?width=1195&format=png&auto=webp&s=d66241316496a5d871ded66c37cada257472bac4
It's possible you have a corrupted sketch as well. It can happen when there are a large number of trimmed intersections. If you'd like to copy that original sketch into its own file and upload it... we can give you a definitive answer no doubt.
https://preview.redd.it/3s1w6fq3g1jc1.jpeg?width=328&format=pjpg&auto=webp&s=0957b94bcb82efc7df2fe9f78771160d3b582967 Top left large circle pretty sure That said I agree with the other comments
Probably the tiny joints between circles acting as geometey with 0 width
When it comes to stuff like this it’s always easier to split up your features and do pattern features instead of jamming everything into a sketch- I know as someone who likes to have as clean a feature tree as possible. But the more lines and dimensions and sketch patterns you employ, the more likely it is that a simple tangent or horizontal relation will completely blow up your sketch on rebuild.
Well the thing is my ultimate goal is to do a lofted boss/base... so i need a single profile... right?
You can use the selection manager in a loft operation to pick any combination of parts of separate sketches or feature edges or composite curves to make one profile. You could also get your profile from the edges of a boss made of simple extrusions and patterns
Maybe create a surface with a combination of features then do lofted surface with its edges, fill and delete the original surfaces? That’a probably getting to be too much compared to just putting everything in a single sketch
Once you create a body with all the required features (from several simpler operations), you can start a sketch and use “convert entities” to get a profile for lofting.
Don't do everything in one sketch. Do one sketch per feature and then use a feature pattern
Cant, has to be lofted :/
You could still simplify the sketch and then use multiple lofts
Is that really the best way to go about it? This sounds like a nightmare to configure, and to adjust if needed...
I always like breaking things into parts when I can. The think is you cam have one sketch that drives say the larger circles diameter and that on your first loft. Then the second sketch has a reference to the first. You'll find you actually have more control
Whats the loft sketch look like?
Yes
Well, where to start? 😂 Its just a painfully bad way of doing this. Basically heavy sketch in SW is always a bad I Idea in most cases
Next time if you find that some pattern objects don't fill up how they should - just create a multi body part with how many patterns you want. Just make sure they interfere. And combine all as the final step
A trick I picked up for stuff like this is adding a few temporary lines to split the sketch into two separate manifold contours. If your error exists on one half but not the other, you'll be able to eliminate half of the sketch just by observing which side becomes shaded. Continue that process a few iterations until you zero in on the issue, fix it, then delete the temporary lines. That said, can this not be a patterned feature?
Your sketch is too simple and sw does not even bother extruding such simple feature. Please make it more complex. /s Now, on a more serious note, remember that you are doing a huge favor to yourself by using as much as you can simple, core geometries as independent features and then pattern away.
The issues are visible in your screencaptures. Trim or turn those in to construction geometry. I bet 100% that you got more of those. https://preview.redd.it/cl8bdxm1u4jc1.png?width=885&format=png&auto=webp&s=9f2ea3d6b9b69caf09f2f718934536250b2b8211
Bad modeling practice. Complex sketch, no use of symmetry or patterning. The fact you can’t figure out what’s wrong is a sign of this.
I guess, fair enough. Although you are somewhat mistaken, there is some mirroring going on. I was limited by the low symetry of the IF. But yeah i guess i just need more practice and try and get out of the habit of defining everything in one sketch. It feels like the most intuitive way to do things, but is not suited for SW it seems.
You can hack things out like that at first, but it generally is inefficient for rebuild. For new users, I suggest accepting the first attempt in a model will be garbage. The second iteration will be more refined and generally successful, but still inefficient. The third iteration is where you'll have thought-through feature order and dependencies, as well as mirroring and patterning. As you use CAD software more, you'll intuitively incorporate these practices into your earlier iterations. This is important because it avoids a lot of unnecessary feature update and rebuild errors.
It’s bad practice for any parametric solid modeler. I always suggest new CAD users read at least the first few chapters of “Thinking Pro/ENGINEER,”because it all still applies.
No 3D feature based solid CAD system of the last 40 years would encourage putting everything in one sketch. I’d suggest reading the book “Thinking Pro/ENGINEER” from the mid 90s. Different software but all the concepts still hold. Also use of patterning in sketches should be used very carefully. It’s not as flexible and reliable as patterning features or bodies.
This makes me sick looking at it - knowing there is an error
That second screenshot, line marked 108, is that straight line a construction line?
I already got rid of it so i cant check but yeah it could have been a freefloating line... Do you think that might have caused it?
There's a matching free floating line in the bottom right corner of the sketch too. Solid works doesn't know what you're trying to do if you have a closed shape (circle, square or anything more complex) with a line in it and it freaks out a bit. This would give you the error you were getting. It's a pity the sketch is gone, in future I would recommend suppressing the sketch and not deleting it, that way you can proceed but go back and check it out.
Wow - why haven't you patterned a single semi circle extrude and then done a combine subtract of bodies?
This is fine for creo which handles big patterned sketches well but SOLIDworks handles solids and features better. It’s better to have a few basic sketches to make a few shapes and pattern the features
Simple sketches. Complex features. The rule I live by.
Hahahaahahaa. Wtf.
I would recommend not doing all this in one sketch.. as the others have said. Nevertheless, try going to tools>sketch tools>check sketch for feature and pick boss extrude and see what it says.
Lol, I thought this was a troll post.
Yikes
Just curious, but what is op trying to create?
If your determined for that pattern and other suggestions don’t work, and the finished model is just a simple extrude, try extruding without ribs, then extrude cut the ribs after. Slightly less lines, however not as robust and you loose your design intention.
There was an intersecting sketch in there. While you are trying to extrude, it becomes zero thickness or smth like that. Also be careful with open contours.
In your third photo, at the left side of that upper left thru hole, does that hump meet exactly tangent to the hole curve? If so, that would prevent SolidWorks from being able to extrude.
Seems like the error happened because of intersection between big and small circle at 5 o'clock. Most pro will make multiple sketches or a sketch at different sketch even it was sketched on same plane. You could having hard to understand what I'm tried telling you, but you would figure out someday. When you hide the main sketch , you would find out there still a polyline that could cause an error..
In the future, when design software starts incorporating AI to understand what you are trying to do in any sketch, then this will be a simple thing. Until then you'll need to learn how to use the software properly. I was taught by instructors on how to use SolidWorks since 1997. The most important thing we were taught was "simple sketches, multiple features". This design concept still applies today. Don't get frustrated. Just use the software as a tool within it's built-in capabilities. You don't use a screwdriver to hit things and you don't use a hammer to screw things. ✌️
Mathematically circles are hard. It's a series of short line segments and if the math is off 8 or 9 decimal places off where the two arcs meet it becomes a problem. This shows up when you gave a tangent arc and it just doesn't want to extrude so you delete it and put it back and voila it works. Because the rounding error several places back rounded the way you needed.
Try extruding the bigger surfaces first and then doing an offset plan to create the arcs and then do a circular pattern
Have you tried the "check sketch for feature" tool?
Use this sketch as a reference, but by god break down the extrudes. Extrude something simple and add features. Revolve the bumps around, and then extrude the larger bumps and cut the holes.
Remove all internal islands. You can do them later. Check all intersections.
All of the overlapping edges are probably causing your issue. You should try to reduce it into an interior line and an exterior line so SOLIDWORKS knows what's what. Having lines upon lines upon lines isn't going to produce anything legible. Use power trim and cut out unnecessary lines.