Yea, easy when you already know what to design. That is the problem with the cad software designers and instructors, They are seeing and approaching problems from a different perspective than a designer - "This is the best way to design this assembly"....... But most creative designers just have a very rough idea in their head when they start. Then the design will grow slowly from blocky parts and grow by adding/removing features/parts hundreds if not thousands of times in the most chaotic order.... Yea, one could redesign everything again and get it clean and optimally structed after this creative phase, But small companies don't have such resources, and the design will be used as it is.
This is a great comment, as I can understand your frustration and am sure others have felt this way as well. I have felt the same way watching people do surfacing Tutorials for SW too. The truth is, you are right, CAD is a terrible iteration and ideation tool. It takes way too long to create even the simplest of geometry, let alone build proper file structure and dependent relationships. However, even though that is true, the solution is not to throw those things out. That would be an excuse for poor CAD practices. Rather, it is to use other, more effective tools for the ideation and conceptualization phase. Moving to CAD only when you can leverage what it does best, relationships and structure. Imagine you are trying to design a new house by building walls and pouring concrete, then half way through you realize the layout isn’t right. It would feel really clunky to have to rip all that out to change the design. In fact, that frustration may cause you to build lighter weight walls, or to try to move the concrete around while it’s still wet. The need for flexibility would create bad practices with those tools because they are being used for a job they are not designed for. Same thing here. You are using CAD tool too early in the process to be utilized properly, therefore you are creating bad practices to try and use the tool for something it is not designed for. On a real-world project for a client, it is very rare that I will touch CAD before I have gone through extensive ideation and industrial design with pen and paper or tablet drawing tools. Keep in mind, I am an engineer, not an artist, so these drawings are often very rough and unsightly. Then, once the client has signed of on a design direction based on the 2D sketches, we move towards CAD, then iterate from there. Often times we will design a CAD model and then find a new design direction, but even then, we will go back to 2D sketching and establish direction before trying to capture the idea in a new model. Also, keep in mind you are watching tutorials on how to CAD, not how to design a product from scratch. You only see “cad software designers and instructors” showing you how to draw stuff they already know, because they are trying to show you how to use the tool, not a documentary on their overall process. To make videos showing how to ideate or conceptualize in CAD would be untruthful to their process and bad practice. Hope this helps clarify some things, feel free to reach out if you have any more questions or comments!
@@forgeproductdevelopment no substitute for pen(cil) & paper, highlighters for ideation! That said, I start with some simple reference goemetry in CAD to establish constraints, key datums, and simple sketches. This because we've all sketched something that "made sense" until you put it to scale... Print rudimentary CAD, sketch to ideate, update the sketches, occassionally add more reference features, lather, rinse, repeat. This also creates a breadcrumb trail.
@@raphaelhamm3853 This is an excellent suggestion as well. We have designed products where there are PCBs and motors, attachment points, or other components that are selected based on previous calculations. Sometimes we import those into CAD early on to get a sense of scale, and export out images to draw over the top of when coming up with designs. I think the heart of the matter is "start with what you have and select the best tool to move your forward given the initial conditions'. Whether that be from COTS components, systems you need to integrate with, mathematical calculations, or a completely blank sheet of paper. Each project is unique and part of the fun of engineering is getting to solve and optimize for those challenges along the way.
On top of this, the storage and creation of manufacturing info, especially when parts are shared between products, makes this utterly unworkable in a manufacturing environment that does any real part re-use. I rarely need my assembly to fully update and push changes in multiple subcomponents, and even when I do, I don't trust software to push the changes properly ready for review.
@jamesbuckle6077 You are right, this would be terrible if you tried to do it this way, but that would be a misuse of the technique. This is primarily for NEW part design. Once the product has been validated and released (ie. is stable), best practice is to freeze or break the relationships, so the parts can exist on their own. By doing this, you can reuse them in future assemblies, just like any other COTS part, without worrying that they would change due to revisions in the parent assembly. Any future changes would be subject to normal ECN processes. I blame myself for the misunderstanding, because I do not cover this part of the workflow in the video. Think of it like this: you would not reuse a part in multiple products that has not been designed yet (and if you were designing a multi use part, this technique would still be the best way to do it, as you could create functional relationships between both assemblies), and once it was designed and ready for incorporation into future work, the design would be stable and therefore locked out to exist on its own. Does this help/make sense?
Thank you immensely. I'm coming into SW from 20 years in Inventor and was wondering how top-down design is done in SW. The other videos I watched wrongly claimed top-down when they were in fact showing middle-out strategies.
Welcome to the dark side haha. The first job I had out of school used Inventor, but I am sure I was terrible at it. How do you do top down in Inventor?
@@forgeproductdevelopment Top down in Inventor is pretty much the same workflow as this. The only difference is you can derive out solids and surfaces from the skeleton part in addition to sketches. I'm sure it's possible in SW as well, I just haven't figured it out yet.
If I wanted to chamfer an edge on the block, and control the chamfer dimensions from the skeleton file, how do I accomplish that? I can't find a way to relate those dimensions. Great video, by the way.
Thank you so much for the kind words! Great question. I would create a global variable for the fillet width inside the skeleton sketch part file. Use that variable as a dimension inside the sketch. Then, create another variable within the part file where the chamfer feature will be created. Next, within the parent assembly, set the part variable to be equal to the skeleton part variable. Lastly, create the chamfer feature and set the width equal to the variable within its part file. Now, whenever you change the dimension inside the skeleton sketch, it will pass the value to the other variable and the feature. Another cool trick, you can dimension previously constrained geometry in a sketch (a derived sketch) and set the new dimension to "driven". This basically creates a dimension that is measuring geometry for you, that you can reference in your equations/features. When the measured geometry changes size, the driven sketch dimensions changes, and updates your equations/features. Both options can work depending on your use case. Keep in mind, daisy chaining dimensions and features like this, especially if it is across multiple parts/files, may cause rebuild issues. I always try to make changes from within the parent assembly, so all parts are open and rebuilding together. Also, "ctrl + Q" will be your friend.
@@forgeproductdevelopment thank you so much! Great answer. Can’t believe you’re still replying to comments this long after it’s been posted. Awesome work
How about insert part the skeleton into sub-parts vs derived sketches? Maybe more warranted for more complex parts / subassemblies, and too much overhead for lots of simple parts?
Inserting a part vs derived sketches is a questions that gets brought up quite a bit. I have not done enough testing between the two to say one should win outright. At this point I would view them as tools to have in the box. Get familiar with both and then pull each one out when you feel like is has the advantage. At this point I would say both are viable, but I am likely biased towards the SS method due to familiarity.
Thanks for doing these type of tutorials, they are great! I feel like almost all of these smart and stable tricks are not practical when you throw in a PDM and a PLM solution in the mix. Having all these references between parts and assemblies will most likely create a revision nightmare if you need to make a minor change and you end up with a lot more work. What are your thoughts on this?
Thank you for your kind words and your thoughtful question! I had a much longer response to this, but think I will save that for a video. The simplest summary of my thoughts is, when designing from scratch, I think it is better to build this type of functionality in to the models, and then break or freeze the references when the files go to be released/put in the vault, then work bottom up. As a designer, I can't imagine not being able to pull in references and build relationships. I feel it saves time when making changes, but also helps error proof the design process by ensuring changes are properly propagated to each part. That said, I am always interested in learning alternative methods. Do you typically design from scratch or are you modifying existing parts and assemblies? When do your designs get entered in to the revision controlled vault? When a part or assembly gets entered in your vault, are external references allowed, or must they all be removed? When you make changes to a component, how do you ensure any affected part is also identified and updated? Thanks again!
What about the fact that your pin and hole are the exact same size? How would you create an offset for tolerance/intended fitment (Press fit or loose fit)?
Great question! I have a few different ways to handle this. The first is drawing two circles, one representing the pin and one the hole. This way you can relate them to each other, (say, maintain .005" interference) no matter the diameter. This works great for specifying exact fits, and clearly showing the diameters and fit within the sketch. In very demanding applications, you can even set the holes and pins tangent to each other, instead of concentric, for added stack up accuracy. The one downside to this is that you can end up with a lot of lines and dimensions in your sketches, which can muddy the waters. The other method I have used is is to use the "move face" feature to prescribe the offset. I use "interference detection" as one of my checks, and then create the offsets for each flagged area. I can use search in the feature tree to find all my offsets too. I find this keeps the sketch clean, but is not as easy to create relations and less obvious what is happening, unless you examine the tree. I tend to use this on non-critical fits or large clearances. Hope this helps! If anyone else has methods they use, feel free to share!
Does your 3D assembly really need exact tolerances in the model? Why not just model everything using the nominal sizes, and only add the tolerances when moving on to the manufacturing step, and just note the fitment on the drawing?
@@denisl2760 A couple of thoughts here. I typically do not set/note tolerances within my sketch dimensions, unless it is a tolerance I know I need to be aware of or am documenting within the model for someone in the future. I know if you use "import dimensions" within drawings the tolerances will come in and be linked, which I do like, but I have not added that trick to my normal workflow yet. When you say "nominal size", do you mean make the model geometry at the middle of the tolerance range you end up specifying on the drawing? If so, this is exactly what I do! You can use either technique above (or any other method you like) to get the geometry where you want. If by "nominal" you mean what I call "line to line", where pin and hole diameters would have coradial/coincident surfaces and the clearance would be made by the tolerances of the print, I do not do this for a few reasons. Mainly, when the model becomes the standard for manufacturing and inspection down the road, programs will typically pull surfaces directly from the CAD and if the model is not at nominal, it will be up to someone else to read the print and make the correction. Likewise, when I send parts to be 3D printed, the printer will need it modeled at nominal for me to have the best accuracy. Does this answer your question?
@@forgeproductdevelopment I guess it depends entirely on what the model will be used for, and the manufacturing process. If its directly used to 3D print then yeah I can see why you'd need to include the tolerances in the model itself. But if its going to be used to create a set of 2d drawings and sent to a machinist, the machinist won't care that your 10.1mm hole and 9.9mm pin are actually drawn as 10.0000mm, as long as there is a note on the drawing giving them the desired tolerance.
@denisl2760 In a shop environment where the machinists work exclusively off of paper drawings (and never query the model for measurements) this may be technically true, but I would still advise against it. Even in this situation it relies on the machinist to calculate by hand every measurement that uses that feature. I would much rather give them nominal dimensions and symmetric tolerances, to guard against errors. Also, since it is impossible to know if, over the life of the the model, it will ever be used in a CAM or inspection program (CMM or scanning), queried for measurements, taken out of context of the drawing, or 3D printed, I would much prefer to know my CAD is nominal than rely on everyone down stream of me to catch the one sided dimension that is buried in a drawing and make the corrections. Hope this isn’t too harsh. To be fair, you are going to know what is best for your shop and workflow.
What about downloaded parts like bushings that won't update as you change the pin size? If you design a whole machine like this your parts have an origin that is somewhere well outside the geometry of the part. Cars are modeled top-down and it's generally a pain work with their parts.
You can move the derived sketch after you create it to align with the parts files origin and planes. Jus use your usual sketch relations to control its location. You should actually be doing this every time, to create fully defined sketches and prevent things from moving unexpectedly, unfortunately I did not show this in this video.
I am planning to do a video comparing layout, skeleton sketch and inserting master parts. I am currently swamped with client work. Hopefully I can get back to it soon.
This is great, thank you! So, let's say i want to add a bit of an offset between these two parts for tolerance. Would it then be better to add a second slightly bigger circle on my "skeleton" sketch, or to use the move face feature on the "block" part?
This is an excellent question! I have found that both can be useful. Generally, if I am creating a non-precise gap, I will sketch line to line and then use the move face command. If I need to precisely define the gap for some reason, (bearings, slip/press fits, snap closures, etc.) I will sketch the gap in, so I can dimension it and see the relationship easier.
Thank you for sharing, great information! Is there a reason that you wouldn't create the skeleton drawings at the assembly level, rather than having that first 'skeleton part' to derive your sketches? By having the 'skeleton part' does this really serve as a way to hide those sketches quickly when your isolating other parts, or is there more to it than that?
That is part of it, but the main benefit is keeping the sketches at the top of the tree. SolidWorks likes to solve the the tree and relationships from the top of the feature tree to the bottom. When you start creating sketches within the assembly file, those sketches and planes get pushed to the bottom of the tree. Also, you can easily use that skeleton sketch part file in other assemblies, allowing the same part file and references to be used concurrently. Hope that helps!
@@fouadelshafey502 Ahh! I took the live stream down. I did not take the time to make a plan for the model and therefore ended up with a disjointed mess of a stream. If you would like me to try again, I am happy to do so.
Hi Josh, first of all greate tutorial, very very useful for me. And I have a little question, when saving all the pieces that we created inside the assembly, wich process is better. Saving them inside the assembly or externally? Wich one is more stable? Thanks
Great question! I do both. Early in the design process, when the design is still undergoing large changes and staying within the engineering team. I will leave everything as a virtual part inside the assembly file. When I go to publish or release individual parts or make drawings, I will save each one out to an external file.
Even though I dislike the insertion of an skeleton part within a part, I think it's more stable than this method of derived sketches. The big disadvantage of this method is that you need to constrain again the derived sketches otherwise you will have a mess in the design and That doesn't make sense. In the other hand inserting a part within a part could decrease the performance of the already lag and inefficient software. But the big advantage it's the access to the sketches and parts without opening the assembly and a more clean environment. Have you tested both methods? If so what's your opinion about it. Thanks for the video it was very clear and accurate. You just missed the section of fully constrain sketches which is a key process for a good design practice.
You are right! Best practice is to constrain the derived sketches, I should have included that. Often in my videos I do not constrain sketches for the sake of time, in this case I should have made an exception. The only constraints you need are to locate and orient the derived sketch within the sketch plane. Any constraint that tries to alter the sketch will fail. As for inserting a part within a part vs the derived sketch method, I have not done enough testing to see which has faster rebuilds. I will try to do some testing and make a video on my results. I would imagine the derived sketches would be faster, as you are importing less information, but the intuitive answer is not always true with SW. I can understand the advantage of having the sketches be editable without opening the assembly, but I would be nervous editing a skeleton sketch without seeing how I am effecting other the parts. In that case, I would likely have the assembly open anyways. Thank you for this thoughtful comment! What workflow do you prefer?
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@@forgeproductdevelopment thanks for your reply. I found the master part absolutely effective and very stable related to sketches, planning and organisation. But I think it makes the software very slow. If I compare it to Autodesk inventor the latest just derives the needed sketches without importing any part. Probably that makes the software faster and rebuilds fantastic. I think because of the problem of accessing the master sketch and constraints I would prefer the master sketch part. Been designing big equipment with that and the accuracy is just perfect. If you make a video comparing both please let me know. All the best
@ I have not had any issues with stability using the derived sketch method, but I would be interested to compare the two. I will have to do some tests and see what I can come up with. Just like Inventor, you can directly convert entities from external parts into a part and use them as references. Though, I have found the stability and rebuild speed not as good as placing either a part or derived sketch within the part file.
@@forgeproductdevelopment please do compare both methods, i'm still relatively new to solidworks and searching for best methods while doing top down modeling, looking forward for that video
@@khalilbahlawan4439 I will try to make this a priority, since so many people seem interested. Since you are new to the software, I would advise trying both and seeing how they perform for you. What technique have you been using?
It feels like your making the Most Basic operation So More Complex than it needs to be… I do understand the intent of Stable Architecture. The one thing I dislike about Solidworks Still after 25 years is How Fragile it is. AutoCAD products are more Robust, but it ain’t easy to learn new CAD package tools sometimes.
Funny Enough I have Built Large Span Steel Bridges in real life,Designed in Solidworks… But none of them are High Enough to Jump off as a Reset on Life.
Yea, easy when you already know what to design. That is the problem with the cad software designers and instructors, They are seeing and approaching problems from a different perspective than a designer - "This is the best way to design this assembly"....... But most creative designers just have a very rough idea in their head when they start. Then the design will grow slowly from blocky parts and grow by adding/removing features/parts hundreds if not thousands of times in the most chaotic order.... Yea, one could redesign everything again and get it clean and optimally structed after this creative phase, But small companies don't have such resources, and the design will be used as it is.
This is a great comment, as I can understand your frustration and am sure others have felt this way as well. I have felt the same way watching people do surfacing Tutorials for SW too.
The truth is, you are right, CAD is a terrible iteration and ideation tool. It takes way too long to create even the simplest of geometry, let alone build proper file structure and dependent relationships. However, even though that is true, the solution is not to throw those things out. That would be an excuse for poor CAD practices. Rather, it is to use other, more effective tools for the ideation and conceptualization phase. Moving to CAD only when you can leverage what it does best, relationships and structure.
Imagine you are trying to design a new house by building walls and pouring concrete, then half way through you realize the layout isn’t right. It would feel really clunky to have to rip all that out to change the design. In fact, that frustration may cause you to build lighter weight walls, or to try to move the concrete around while it’s still wet. The need for flexibility would create bad practices with those tools because they are being used for a job they are not designed for. Same thing here. You are using CAD tool too early in the process to be utilized properly, therefore you are creating bad practices to try and use the tool for something it is not designed for.
On a real-world project for a client, it is very rare that I will touch CAD before I have gone through extensive ideation and industrial design with pen and paper or tablet drawing tools. Keep in mind, I am an engineer, not an artist, so these drawings are often very rough and unsightly. Then, once the client has signed of on a design direction based on the 2D sketches, we move towards CAD, then iterate from there. Often times we will design a CAD model and then find a new design direction, but even then, we will go back to 2D sketching and establish direction before trying to capture the idea in a new model.
Also, keep in mind you are watching tutorials on how to CAD, not how to design a product from scratch. You only see “cad software designers and instructors” showing you how to draw stuff they already know, because they are trying to show you how to use the tool, not a documentary on their overall process. To make videos showing how to ideate or conceptualize in CAD would be untruthful to their process and bad practice.
Hope this helps clarify some things, feel free to reach out if you have any more questions or comments!
@@forgeproductdevelopment no substitute for pen(cil) & paper, highlighters for ideation!
That said, I start with some simple reference goemetry in CAD to establish constraints, key datums, and simple sketches. This because we've all sketched something that "made sense" until you put it to scale...
Print rudimentary CAD, sketch to ideate, update the sketches, occassionally add more reference features, lather, rinse, repeat. This also creates a breadcrumb trail.
@@raphaelhamm3853 This is an excellent suggestion as well.
We have designed products where there are PCBs and motors, attachment points, or other components that are selected based on previous calculations. Sometimes we import those into CAD early on to get a sense of scale, and export out images to draw over the top of when coming up with designs.
I think the heart of the matter is "start with what you have and select the best tool to move your forward given the initial conditions'. Whether that be from COTS components, systems you need to integrate with, mathematical calculations, or a completely blank sheet of paper. Each project is unique and part of the fun of engineering is getting to solve and optimize for those challenges along the way.
On top of this, the storage and creation of manufacturing info, especially when parts are shared between products, makes this utterly unworkable in a manufacturing environment that does any real part re-use. I rarely need my assembly to fully update and push changes in multiple subcomponents, and even when I do, I don't trust software to push the changes properly ready for review.
@jamesbuckle6077 You are right, this would be terrible if you tried to do it this way, but that would be a misuse of the technique.
This is primarily for NEW part design. Once the product has been validated and released (ie. is stable), best practice is to freeze or break the relationships, so the parts can exist on their own. By doing this, you can reuse them in future assemblies, just like any other COTS part, without worrying that they would change due to revisions in the parent assembly. Any future changes would be subject to normal ECN processes. I blame myself for the misunderstanding, because I do not cover this part of the workflow in the video.
Think of it like this: you would not reuse a part in multiple products that has not been designed yet (and if you were designing a multi use part, this technique would still be the best way to do it, as you could create functional relationships between both assemblies), and once it was designed and ready for incorporation into future work, the design would be stable and therefore locked out to exist on its own.
Does this help/make sense?
Thank you immensely. I'm coming into SW from 20 years in Inventor and was wondering how top-down design is done in SW.
The other videos I watched wrongly claimed top-down when they were in fact showing middle-out strategies.
Welcome to the dark side haha. The first job I had out of school used Inventor, but I am sure I was terrible at it. How do you do top down in Inventor?
@@forgeproductdevelopment Top down in Inventor is pretty much the same workflow as this.
The only difference is you can derive out solids and surfaces from the skeleton part in addition to sketches. I'm sure it's possible in SW as well, I just haven't figured it out yet.
How do you structure your top down models?
Great video!
I found this video in a search to learn more on inserting master parts, will be cool to see a video about that as welll
Thanks, can you elaborate on what you mean by "inserting master parts"?
If I wanted to chamfer an edge on the block, and control the chamfer dimensions from the skeleton file, how do I accomplish that? I can't find a way to relate those dimensions. Great video, by the way.
Thank you so much for the kind words! Great question. I would create a global variable for the fillet width inside the skeleton sketch part file. Use that variable as a dimension inside the sketch. Then, create another variable within the part file where the chamfer feature will be created. Next, within the parent assembly, set the part variable to be equal to the skeleton part variable. Lastly, create the chamfer feature and set the width equal to the variable within its part file. Now, whenever you change the dimension inside the skeleton sketch, it will pass the value to the other variable and the feature.
Another cool trick, you can dimension previously constrained geometry in a sketch (a derived sketch) and set the new dimension to "driven". This basically creates a dimension that is measuring geometry for you, that you can reference in your equations/features. When the measured geometry changes size, the driven sketch dimensions changes, and updates your equations/features.
Both options can work depending on your use case. Keep in mind, daisy chaining dimensions and features like this, especially if it is across multiple parts/files, may cause rebuild issues. I always try to make changes from within the parent assembly, so all parts are open and rebuilding together. Also, "ctrl + Q" will be your friend.
@@forgeproductdevelopment thank you so much! Great answer. Can’t believe you’re still replying to comments this long after it’s been posted. Awesome work
@@akaZ__ You are very welcome. It is a lot better than waiting on me to make a new video haha
How about insert part the skeleton into sub-parts vs derived sketches? Maybe more warranted for more complex parts / subassemblies, and too much overhead for lots of simple parts?
Inserting a part vs derived sketches is a questions that gets brought up quite a bit. I have not done enough testing between the two to say one should win outright. At this point I would view them as tools to have in the box. Get familiar with both and then pull each one out when you feel like is has the advantage. At this point I would say both are viable, but I am likely biased towards the SS method due to familiarity.
Thanks for doing these type of tutorials, they are great!
I feel like almost all of these smart and stable tricks are not practical when you throw in a PDM and a PLM solution in the mix. Having all these references between parts and assemblies will most likely create a revision nightmare if you need to make a minor change and you end up with a lot more work. What are your thoughts on this?
Thank you for your kind words and your thoughtful question!
I had a much longer response to this, but think I will save that for a video. The simplest summary of my thoughts is, when designing from scratch, I think it is better to build this type of functionality in to the models, and then break or freeze the references when the files go to be released/put in the vault, then work bottom up. As a designer, I can't imagine not being able to pull in references and build relationships. I feel it saves time when making changes, but also helps error proof the design process by ensuring changes are properly propagated to each part.
That said, I am always interested in learning alternative methods. Do you typically design from scratch or are you modifying existing parts and assemblies? When do your designs get entered in to the revision controlled vault? When a part or assembly gets entered in your vault, are external references allowed, or must they all be removed? When you make changes to a component, how do you ensure any affected part is also identified and updated? Thanks again!
What about the fact that your pin and hole are the exact same size? How would you create an offset for tolerance/intended fitment (Press fit or loose fit)?
Great question! I have a few different ways to handle this.
The first is drawing two circles, one representing the pin and one the hole. This way you can relate them to each other, (say, maintain .005" interference) no matter the diameter. This works great for specifying exact fits, and clearly showing the diameters and fit within the sketch. In very demanding applications, you can even set the holes and pins tangent to each other, instead of concentric, for added stack up accuracy. The one downside to this is that you can end up with a lot of lines and dimensions in your sketches, which can muddy the waters.
The other method I have used is is to use the "move face" feature to prescribe the offset. I use "interference detection" as one of my checks, and then create the offsets for each flagged area. I can use search in the feature tree to find all my offsets too. I find this keeps the sketch clean, but is not as easy to create relations and less obvious what is happening, unless you examine the tree. I tend to use this on non-critical fits or large clearances.
Hope this helps! If anyone else has methods they use, feel free to share!
Does your 3D assembly really need exact tolerances in the model? Why not just model everything using the nominal sizes, and only add the tolerances when moving on to the manufacturing step, and just note the fitment on the drawing?
@@denisl2760 A couple of thoughts here.
I typically do not set/note tolerances within my sketch dimensions, unless it is a tolerance I know I need to be aware of or am documenting within the model for someone in the future. I know if you use "import dimensions" within drawings the tolerances will come in and be linked, which I do like, but I have not added that trick to my normal workflow yet.
When you say "nominal size", do you mean make the model geometry at the middle of the tolerance range you end up specifying on the drawing? If so, this is exactly what I do! You can use either technique above (or any other method you like) to get the geometry where you want.
If by "nominal" you mean what I call "line to line", where pin and hole diameters would have coradial/coincident surfaces and the clearance would be made by the tolerances of the print, I do not do this for a few reasons. Mainly, when the model becomes the standard for manufacturing and inspection down the road, programs will typically pull surfaces directly from the CAD and if the model is not at nominal, it will be up to someone else to read the print and make the correction. Likewise, when I send parts to be 3D printed, the printer will need it modeled at nominal for me to have the best accuracy.
Does this answer your question?
@@forgeproductdevelopment I guess it depends entirely on what the model will be used for, and the manufacturing process. If its directly used to 3D print then yeah I can see why you'd need to include the tolerances in the model itself. But if its going to be used to create a set of 2d drawings and sent to a machinist, the machinist won't care that your 10.1mm hole and 9.9mm pin are actually drawn as 10.0000mm, as long as there is a note on the drawing giving them the desired tolerance.
@denisl2760 In a shop environment where the machinists work exclusively off of paper drawings (and never query the model for measurements) this may be technically true, but I would still advise against it. Even in this situation it relies on the machinist to calculate by hand every measurement that uses that feature. I would much rather give them nominal dimensions and symmetric tolerances, to guard against errors.
Also, since it is impossible to know if, over the life of the the model, it will ever be used in a CAM or inspection program (CMM or scanning), queried for measurements, taken out of context of the drawing, or 3D printed, I would much prefer to know my CAD is nominal than rely on everyone down stream of me to catch the one sided dimension that is buried in a drawing and make the corrections.
Hope this isn’t too harsh. To be fair, you are going to know what is best for your shop and workflow.
What about downloaded parts like bushings that won't update as you change the pin size? If you design a whole machine like this your parts have an origin that is somewhere well outside the geometry of the part. Cars are modeled top-down and it's generally a pain work with their parts.
You can move the derived sketch after you create it to align with the parts files origin and planes. Jus use your usual sketch relations to control its location. You should actually be doing this every time, to create fully defined sketches and prevent things from moving unexpectedly, unfortunately I did not show this in this video.
Hi I was wondering if you could maybe explain the difference between skeleton sketch modeling vs assembly layout?
I am planning to do a video comparing layout, skeleton sketch and inserting master parts. I am currently swamped with client work. Hopefully I can get back to it soon.
This is great, thank you!
So, let's say i want to add a bit of an offset between these two parts for tolerance. Would it then be better to add a second slightly bigger circle on my "skeleton" sketch, or to use the move face feature on the "block" part?
This is an excellent question! I have found that both can be useful. Generally, if I am creating a non-precise gap, I will sketch line to line and then use the move face command. If I need to precisely define the gap for some reason, (bearings, slip/press fits, snap closures, etc.) I will sketch the gap in, so I can dimension it and see the relationship easier.
Hi! Is it possible to work like that in SW for Makers?
I have not used it, but if it is just a low cost license of the main desktop software, then yes.
Thank you for sharing, great information! Is there a reason that you wouldn't create the skeleton drawings at the assembly level, rather than having that first 'skeleton part' to derive your sketches? By having the 'skeleton part' does this really serve as a way to hide those sketches quickly when your isolating other parts, or is there more to it than that?
That is part of it, but the main benefit is keeping the sketches at the top of the tree. SolidWorks likes to solve the the tree and relationships from the top of the feature tree to the bottom. When you start creating sketches within the assembly file, those sketches and planes get pushed to the bottom of the tree. Also, you can easily use that skeleton sketch part file in other assemblies, allowing the same part file and references to be used concurrently. Hope that helps!
Sir where can I find your last tutorial?
Which one are you looking for? You should be able to find them all here: th-cam.com/channels/3k2BrjNyNgPqKRWS_2Q0hQ.htmlvideos
@@forgeproductdevelopment I'm looking for the live tutorial yesterday
@@fouadelshafey502 Ahh! I took the live stream down. I did not take the time to make a plan for the model and therefore ended up with a disjointed mess of a stream. If you would like me to try again, I am happy to do so.
@@forgeproductdevelopment that's very kind of you .I don't want to bother you
Hi Josh, first of all greate tutorial, very very useful for me.
And I have a little question, when saving all the pieces that we created inside the assembly, wich process is better. Saving them inside the assembly or externally? Wich one is more stable?
Thanks
Great question! I do both. Early in the design process, when the design is still undergoing large changes and staying within the engineering team. I will leave everything as a virtual part inside the assembly file. When I go to publish or release individual parts or make drawings, I will save each one out to an external file.
@@forgeproductdevelopment all right, perfect I see that way to work pretty consistent.
Thanks for your reply.
good job，keep moving on
Thank you!
Even though I dislike the insertion of an skeleton part within a part, I think it's more stable than this method of derived sketches.
The big disadvantage of this method is that you need to constrain again the derived sketches otherwise you will have a mess in the design and That doesn't make sense.
In the other hand inserting a part within a part could decrease the performance of the already lag and inefficient software. But the big advantage it's the access to the sketches and parts without opening the assembly and a more clean environment.
Have you tested both methods? If so what's your opinion about it.
Thanks for the video it was very clear and accurate. You just missed the section of fully constrain sketches which is a key process for a good design practice.
You are right! Best practice is to constrain the derived sketches, I should have included that. Often in my videos I do not constrain sketches for the sake of time, in this case I should have made an exception. The only constraints you need are to locate and orient the derived sketch within the sketch plane. Any constraint that tries to alter the sketch will fail.
As for inserting a part within a part vs the derived sketch method, I have not done enough testing to see which has faster rebuilds. I will try to do some testing and make a video on my results. I would imagine the derived sketches would be faster, as you are importing less information, but the intuitive answer is not always true with SW.
I can understand the advantage of having the sketches be editable without opening the assembly, but I would be nervous editing a skeleton sketch without seeing how I am effecting other the parts. In that case, I would likely have the assembly open anyways.
Thank you for this thoughtful comment! What workflow do you prefer?
@@forgeproductdevelopment thanks for your reply.
I found the master part absolutely effective and very stable related to sketches, planning and organisation. But I think it makes the software very slow.
If I compare it to Autodesk inventor the latest just derives the needed sketches without importing any part. Probably that makes the software faster and rebuilds fantastic.
I think because of the problem of accessing the master sketch and constraints I would prefer the master sketch part. Been designing big equipment with that and the accuracy is just perfect.
If you make a video comparing both please let me know.
All the best
@ I have not had any issues with stability using the derived sketch method, but I would be interested to compare the two. I will have to do some tests and see what I can come up with.
Just like Inventor, you can directly convert entities from external parts into a part and use them as references. Though, I have found the stability and rebuild speed not as good as placing either a part or derived sketch within the part file.
@@forgeproductdevelopment please do compare both methods, i'm still relatively new to solidworks and searching for best methods while doing top down modeling, looking forward for that video
@@khalilbahlawan4439 I will try to make this a priority, since so many people seem interested. Since you are new to the software, I would advise trying both and seeing how they perform for you. What technique have you been using?
It feels like your making the Most Basic operation So More Complex than it needs to be… I do understand the intent of Stable Architecture. The one thing I dislike about Solidworks Still after 25 years is How Fragile it is. AutoCAD products are more Robust, but it ain’t easy to learn new CAD package tools sometimes.
nice thanks
how to save it all differently
Do you mean how to save out each file individually, rather than as virtual components within the assembly?
@@forgeproductdevelopmentyes
Ten Minutes in and You Still Haven’t drawn a Cube with a Hole or a Peg.
Блин, хорошая у вас тюрьма, был бы в Теннесси обязательно какой-нибудь закон нарушил, чтобы также в солиде развлекаться
Funny Enough I have Built Large Span Steel Bridges in real life,Designed in Solidworks… But none of them are High Enough to Jump off as a Reset on Life.