Name: SOLIDWORKS Tips & Tricks: Mastering Left & Right-Hand Parts the Smart Way
Uploaded: 2026-04-30T18:00:10.422Z
Duration: 42 min 8 s
Description: SOLIDWORKS Tips & Tricks: Mastering Left & Right-Hand Parts the Smart Way

Transcript for "SOLIDWORKS Tips & Tricks: Mastering Left & Right-Hand Parts the Smart Way": Hi, everyone. Thank you for joining today. So we'll be walking through the tips and tricks to master left hand and right hand parts the smart way. Hi. I'm Rishabh Sharma, and I'm located in Kitchener, Canada. And I'd love to know from where you guys are joining in the chat box. So I'm a robotics engineer by education and an elite application engineer by profession. And I work closely with engineers across industries to solve modeling challenges, streamline their workflows, and avoid any pitfalls they have to that slow down their projects. So for instance, the large assemblies, PDM, and so on. So in the next thirty minutes, we'll be going to talk about something that seems simple but can create major headache if done wrong. So that is your opposite hand design in SOLIDWORKS. Let's start with why this even matters. So opposite hand parts shows up everywhere in real engineering. Right? Like brackets, linkages, and closures, but many teams still remodel them manually, which leads to them errors, inconsistent drawings, and waste of engineering time. So today, I will show you how to eliminate all all of that using the clean industry specific standards and workflows. So my goal for today will be to build an opposite hand part fast, clean, and industry correct. I have opened a quick poll that you can see between the chat and the q and a. So this poll is just for me to understand where my current audience is. So it's how do you currently create opposite hand parts. Are you use, like, creating them manually? Are you using the mirror features, assembly mirrors? Or you can say, hey. I'm not sure. I'm here to learn. So please go and submit your polls quickly. There is option. You can submit them, like, multiple answers as well. And, basically, this will basically help me to understand where my current audience is. So no judgment. Most people still remodel them manually. Right? So feel free to submit your poll. Alright. I can see some results coming in. Nice. Nice. Okay. So let's start further. I can see where where most of you are coming from, so that's nice. Let's move to the agenda for today. So today, in this session, in this webinar, I'll be talking about the part level mirroring, then move into the assemblies, and then sheet metal. And finally, I will wrap up with the drawing standards and best practices. So you can feel free to drop your questions in the q and a tab, and I'll try to answer them by the end of the webinar. So tip number one for today is part level mirroring. And here we have I have listed two methods for part level. One, I'll be using with the configurations where I have the same file name but two different configurations. And then I will talk about, creating a separate opposite hand file. And why I'm saying separate? Because this is the fastest way to clean create a clean opposite hand parts. And it's not a feature mirror. It's basically a body level mirror. That's all works best for you, and it also transfer all the information from your original part to the opposite hand version of it along with the dimensions, custom properties. So let's take a look in SolidWorks. Alright. Let's start with the first method, creating left hand and right hand part versions inside the same part file using the configurations. So here I am using this, bracket here where you can see I have a different size of holes all around it along with the tabs that is coming in the upper direction have a different height. So definitely, if I create the opposite version of it, that will be a distinct one. So to start with, as you all know, we need a reference plane. First, I will go with configuration. Sorry. Let's do that. And if you see on the configuration tab, I have renamed my default to left hand. Add a new configuration, right hand, our edge. Click okay. So next step is I would need a plane there. So let's go to the feature tree and select the plane that I'll be using to create the opposite hand version of it. So as you can use the standard planes, but here I'm using a custom created reference plane. Click on that, and the next step is you have to click on insert, or you can use your shortcut menu to enable the mill command. So by default, SOLIDWORKS will pick up your reference plane. And as I said, this is not a face or feature mirror. I'll be doing the body level mirror. So select your body from the graphics area. Make sure to uncheck uncheck the merge solids because I want two separate bodies in in here. So as you do that, now I have two separate bodies in my graphics area, and I'm gonna remove the left hand one from the right hand configuration. To do that, I will simply press the s key shortcut from my keyboard and search the command delete key body. So this is the best way to search for a command, and you can directly select the one that you want to remove from this configuration. And SOLIDWORKS will remove that for you by adding a new feature. So now if I switch my configuration, the left hand will show me the left hand version of it. The right hand version configuration will show me the right hand version of it. Right? So this is one way of doing it. And in this case, your configurations are under the same name. Right? Next one is, about the second method. So for the second method, we will have a separate file, and this is best for the industry practices also. So in that case, again, as you all know, we need a reference plane. So I've used the same part with same holes, no different there. And from my feature tree, again, I will go ahead and select the reference plane. So when you when you click on the reference plane, this time, we are not going to select any configuration or we are not going to come put any commands. So this time, we are directly going to insert button and add the mirror part command there. So this is a prerequisite. You have to select the reference plane first, then only this mirror part will appear. Otherwise, this is grayed out. So when you click on the mirror part, it will automatically show you the template that you would like to use, and you can select it. Click okay. And when you do that now on the top, you can see it's showing a new part number, new part name, and I can transfer all the information from my original part to the left hand configuration. Or if you're working right hand, so you can transfer all that information to your newly created part. So here I'm going to pick axis and plane along with the other selections and, most importantly, the link. So this is my understanding if I want to maintain the, reference, maintain the link with the original, or I want to make it independent. So in this case, I am going to make it, in the make maintaining the link between the new and the old one, and then it will ask me for the units, which units I want to prefer. And once doing it, now you can see, SOLIDWORKS has created a mirror version of my bracket, and it has also copied all that information from my original part to the, right hand mirror part. So as you can see in the feature tree also, it says, the method is derived middle part. And if I expand the feature tree, it doesn't have a long feature tree. It has just one solid body along with few planes that I have copied over. I'll tile my screen vertically. I'll make some room here to show you, some changes here. So right now, let's make it zoom to fit to screen so that you can see the changes. So this is exactly the opposite hand version of it with all the holes aligned as needed. Right? So this this method is, I would say, the best for creating a manufacturing ready part. And the best part is I haven't broke the reference, so I will go and edit my main sketch there. So let's go and change the diameter from six to eight. And once you do that, click eight and then okay. Save it. Once you save and rebuild it, your other part other model will automatically update. So you don't have to worry about, hey. I have to go to the other left hand version of it and to update the dimension there, or I have to make some changes in the custom properties or the planes so everything remains same. So let me rebuild the model, and now you can see it's diameter eight there. So the changes that you make on one side, that will automatically update on the another version of it. So this is ideal for when you have you need a unique part number, you need a separate drawing, and you need, you need to route each part through either PDM or your approval process because in that case, you need a separate part for left hand and for right hand. You cannot use the configurations in that case. Right? So these are the two methods. Let me quickly go through a takeaway from here. Configurations, yes. That is good, for internal discussions, community discussions, or if you want to do a quick comparison between your models for both left hand and right hand versions. It stays on the same file, and it's not ideal for PDM or I would say approval process if your part is going through a if your both parts have a different part numbers. If they are having same part numbers, then I would say configuration is the best way to go ahead. Whereas your second method is best for creating a clean opposite end part and where you need a separate part. As I said, the second method is best to create a separate part number for manufacturing. So this keep your design intent intact and avoid any rebuild issues. Right? So you don't have to worry about, oh, I have to go to the previous model to make the changes or I have to switch between the drawings to make the updates. So once your model is updated, as it is linked, that will update automatically. Great. So that covers the part level approach. Let's take it a step further and look at how assemblies can automatically generate the opposite hand components. So with correct orientation and naming. So that's the key here. Alright. Before we begin, let's do a fun exercise here. I have used an object from my office, and I want you to guess what it is. Type your guesses in the chat, and the first person who gets it right will get a shout out at the end of the webinar. So I'll give you everyone a few seconds. Perfect. I can already see some guesses coming in. Alright. So the object I used is a chair. I have seen a lot of people have given the correct answers, so that's good. And when you see the chair, you must be wondering why does this chair only have one arm? Where's the other one? So, exactly, that's what we are going to solve today, and I'll show you how to use the opposite hand version in SOLIDWORKS to create the missing arm, along with the back support, hinges, screws, all of them together. So this is my chair that I have used. And if you see look at the feature tree, let's go and open my main assembly. So this is my main assembly. And in here, as you can see, the left arm is there. The grip is there. The back support is there. But the hinges are there, but not they are not available on the other side of it. Right? So let's see how we can create them using the, mirror component command and create the opposite version of them. Perfect. So in this case, again, as you know, for the mirror commands, we need a plane. So I'll choose the right plane as it passes through the center of my chair. And then using my s key shortcut from the keyboard, I will enable the mirror component command. So SolidWorks will automatically pick up my right plane, and all I need to do is just select the components that I want to mirror. So either you can select from the fly out feature tree or you can select from the graphics area. So I will choose them one by one, selecting from the screws, the hardware, the the hinge, the arm, the grip, and the backside support. So once you do all these selections, what people miss out is they directly go and click on the green check mark to create the middle part. But what a lot of people miss is there is an arrow on the right hand side. So you have to go and click on that arrow, and this will open a lot of options or a lot of, things that you can change or manipulate in your model. So now I have option to mirror type. I can, mirror it about the bounding box. I can mirror it about the, mass. I can mirror it about the origin. So I can choose it. So in this case, I'll be going through the bounding box. And if you look at next option, it shows you all the selected components that you have selected in the previous step. And once you click on them, it will show you in the preview tab right there. So you can see. And next, it shows gives you an option saying, hey. You point a x flip direction, y flip direction, and or you need to create opposite hand version of it. The best part is SOLIDWORKS has also given us an option to isolate them one by one. So if you isolate it, you can see the correct orientation of your model. So for my arm grip, the backside support but let me rotate the model here so that I have a better view, what I'm doing. So when I click on the arm, I can see they are positioned correctly, but my back support is not. So the orientation matters a lot when you are doing like, creating the opposite version in the assembly. So I've checked not other versions are working for me, but I switch it to opposite hand, and it aligns perfectly with my other side support. I will uncheck the isolate option to make sure that everything looks good. All the models look perfectly, fine, how they should be aligned in my assembly. And once you do that, again, you have to click the next arrow because this will give you a few more options. As you can see here, Solvos has automatically filter out the components. Those are in the opposite hand version, so you don't have to do anything there. And along with that, it also gives you an option to save your files. So either you can use the derived configuration or create a new file. For this one, I'll create a new file, and I will add a prefix there. So you have an option to add either a prefix, either suffix, or or you can add a give it a custom name that you would like to. Right? So I will go with the prefix, and I will write r h. That is for right hand. And just below that, you will see the changes the new name of my other hand version. So that is RHDashB Side Dash0012. So whatever name you will give above, you will see the results there. And then by clicking on the three dots, you can open your, save option where you want to save it. My suggestion is you can create a separate folder where you can save your opposite version or you can save it in the same file. And when you hover on those three dots, you can still see the location where your file is being saved once it is created because all routes will automatically save them. And then next, you guys, I'm pretty sure, are, familiar with the screen again. So when you are creating an opposite hand version, again, you can transfer all the information from your original part to your to your newly created, right hand version. So as you can see, I have some selections. I'm going to uncheck the cosmetic threads because there is no thread in it. But I will check the custom properties, make your selections, and then, again, you have option to make it independent or you want to maintain the, link between the both the components. So I will again leave it open. Alright? The only thing is, in the next presentation, I will show you how what happens if you break the link so you get a better idea if you choose to keep the link or break the link. Now I will click okay and select my template and click okay again. And you will notice SOLIDWORKS will create the other version of my arm right there in front of me. Right? I will rotate it so that I can take a closer look. It looks good, but I believe the appearance is different. So let's update the appearance so it looks same. So I will copy the appearance from the other side and paste it on my newly created arm back support, and rest is good. Now I will change the display state. So I don't want to see the edges there. Perfect. And if you zoom to fit, your grip is also copied there. So during this process, what SOLIDWORKS did? So SOLIDWORKS has created a mirror component. So SOLIDWORKS has applied a mirror component command here. And let's talk about what what SolidWorks did in that area. So if you just look at the mirror component command, all the components are there, but most of them are just flipped by x axis or y axis. But if you notice, the last one that says r h dash b side, so this is the newly created opposite hand version, and this is a separate file again. Right? So you can simply select the, you can check the description comp, name of the component. You can check the path. It is coming from a whole different location. Right? So now you have two components in your assembly. One is b side that we are using for left hand, and then the other one is your right hand b side that is for the right side. And now I will go ahead and save it. So once you save it, let's come back to the main assembly. Press control q for the force rebuild, and you can see my updated chair is like, my the other side of my arm is updated. And I want to look at the custom properties because if you remember, I have copied over the custom properties for this, for this site support, and it's still linked with the left hand side. So I would like to go and update the custom name description name there. So even if you're having a material, you have the finish, you have drawn by anything. Over here, you can also copy over all that information as well. In my case, I have just one description, so I will just update it, save it, go back to my top level assembly, and my design work on the solid wood side is complete. But let's do a quick comparison on drawing for the bill of material, how your new conference will look like over there. So let's open up a new template, like new drawing template, and I will insert a isometric view for the chair. So once you insert the isometric view, let's change the display style, and I would like to change the scale as well. So one ratio 20 to one ratio 10. Looks good. I would also like to change this display state. Yeah. Change it to without edges. Click okay. There you go. So once it is there now, let's add a bill of materials to see the changes. So right click on it, the view, bill of material. I'm using the standard SOLIDWORKS template for the bill of material. Perfect. If you look closely, the line item nine is basically your left hand side support as I can see in the description. Let me expand it so that you can see the preview of your model as well. Right? So line item nine is your left hand support. And if you look at line item 15, that is your right hand support along with the review of your model. So that's how you can use the component, like assembly mirror components where you can create the opposite hand versions. And these are they both appears on separate items in the bill of material along with its own name and the file path that wherever you save it, either inside the PDM or or you can save it on the local drives. It's up to you. So what we have learned here is, when you apply the mirrored component command, do not hit the green check initially. Make sure you click the arrow on the right hand side to explore more options of mirroring your components in the assembly. I have also highlighted the box over there, the icon that is used for creating the opposite hand version. The rest of them are just the x axis or y axis flip. So you can browse them, but for to create the opposite hand version, this is the icon. And when you finalize the component, you finalize the orientation, everything looks good, then make sure you can choose which information that you want to transfer from your original part to the opposite hand version. Perfect. Now let's move to the tip number three, sheet metal mirroring. So I would say sheet metal is where mirror really shines. So you get a flat pattern transfer, bend nodes, grain directions. So everything manufacturing needs. Right? So why I'm saying because this is the all information when you create a mirror part manually. For the another side, maybe your grain direction is different. Maybe your main nodes are different. So when you copy it over, every information will come along with it. And, basically, you can like, getting these things wrong can lead up to, like, expensive your manufacturing mistakes. So let's walk through it. And in this exercise, I'll be using a sheet metal enclosure. So here's my sheet metal enclosure. And as you can see on the left hand side in the feature tree, all the sheet metal commands are applied. And in this enclosure, I have some cutouts on the right hand side, and I want to create an opposite hand version with those cutouts. Right? So in this case, I'm again going to use the insert middle part command. So in that case, I'll look for the standard planes, but let's create a new plane. So using my control key key control button on the keyboard, I can simply drag my existing plane, one of the corner of my existing plane, and you can quickly create the plane using this shortcut key. Click okay. I'll place them at a 200 distance and align them, rename it to reference plane so that it looks good in the assembly feature tree. I will again go to insert, mirror part, select the template, and click okay. Now this is the key that you have to look here. So this time, I'm converting, creating a mirror part for the sheet metal. So I have to make sure I have I will check the sheet metal information so it capture all the information for you. In case that is grayed out for you, all you need to do is click the break link to the original part and uncheck it. So that will come up. That will give you an option to select the sheet metal information. This is a quick tip that you will see in your previous models that this is straight out. So, yeah, let's select the sheet metal information, and this time, I'm going to break the link. So I'm not maintaining any link with my original part. I will break the link. And now in the feature tree, you can see all the tree is copied over for me. So it's not this time, it's not just a small feature tree. It's a complete feature tree with all the features that I have on my original part, and I'm gonna delete the folder from here so you can look at closely. All the tabs, edge flanges. So what SolidWorks did different here is when you have created a new file, SolidWorks has added a body move copy command. So if I suppress that, you will notice my model is going back to the original position. And if I unsuppress it, you will see the change there. So SolidWorks not only copied your part to a new level, it also converted all the information. It also copied or transfer your all the information from original file to this file. Right? So let's do a quick comparison again between the two files. So on the right hand side, you can see my original file that has the cutouts on the left hand side and one on the right. On on the other side, you can see a newly created part that has the cutouts on the other side. And if I do the flattened view, you can see the bounding box length, width, cutouts, they all are same. So cutouts are on the left hand side and right hand side. So I haven't created this part manually. I just used the mirror part command to create it. Right? And this is best because it transfer all the information. Why I'm repeating this? Because a lot of people draw this again and then miss out with the sheet metal information there. Let me show you quickly. When I do a right click and go to properties, you can see the bounding box length, width, thickness, material we are using, how many cutouts are there. So all the information is carried over from your original part to the, opposite hand version of it. Right? So everything is preserved. You don't have to recreate the in the enclosure or manually rebuild the flat patterns. So this is a massive time saver, I would say, to ensure consistency between your left hand and your right hand portions. So let's do a quick change. If you remember, I break the link when I was creating the opposite hand version. So I'm going to make changes here. I will open the mirror command and add a cutout to mirror on the opposite side. So cut extrude four is there and click okay. So what you will notice now on the fixed face, I have two more cutouts. Let me show you the normal view of it. So if I click the control eight for the shortcut key, and now you can see there are a few more cutouts. But if you look at your original part, there is no changes to it. So if you maintain the link, you make the change in one, all things are updated. If you break the link, that will only update your base profile. And now if I show you the flat, pattern of them, you can simply see the changes that we have made on the newly created opposite hand version is there, and the other one remains the same. No changes over there. Right? Yep. Let's see what are the takeaways from this. So I would say this is the one of the most reliable ways to create your opposite hand sheet metal parts without introducing your errors. So why I'm saying without introducing because it it copies your flat pattern, it copies your bend notes, It it it gives you an option to independently edit your feature tree as well for the copied over. Because, like, in the past, a lot of customers ask me, hey. We can use this, but we still need a feature tree to make the changes on it. So this is the best way. You can break the link, and then, everything is copied over. You can make the independent changes on new new files or the opposite hand versions of it. So zero risk of mismatch manufacturing details. Alright. Let's go to the next one that is your, drawings, drawings and industry standards. So in this, I will be basically talking about the how you can create drawings from here instead of copying them manually or making them duplicate. So middle parts automatically carry over all the dimensions and mid model items. Right? So we just saw that. So I'll show you how to add the left hand and right hand properties and the standard node for clarity in your drawing. Right? Because when your model is having all the information, you don't have to overwrite your drawings just to show them. Because if there is a revision or if there is a change, that won't update automatically in the drawings, and that leads to the manufacturing errors or the cost to the company. Alright. Let's jump to Solvox screen here. And to start here, I have opened my and same I have used the same component, the enclosure that we recently created. So this is the left hand version of it where you can see, the cutouts are on the left hand side, and I will quickly open the drawing for this to show you. Okay. I have I have randomly created the drawing. So this is not exactly the manufacturing drawing. Just to trying to show you that you can draw the same as quick as you can. So in this drawing, I have also added three standard views. Along with that, if you look at the title block, all the information is coming directly from my model reference referencing it saying description as left hand enclosures. I have also added a isometric view, flat pattern, along with a bend note, bend table, and sheet metal properties on the top. Even though to highlight, I have added a note at the bottom saying this is the left hand version of my this part. So this will give the more clarity to the shop floor guys so they know, okay. This is the left hand version of the enclosure. This is the part number. And now, now I will close this down, and let's see how you can create this similar drawing with your opposite hand version. So what I'm gonna do here is I will switch to the opposite hand version that we have created. So that named as e n r enclosure right dash two one zero zero. As you can see, the name of the file. Now the if you notice, the cutouts are also on the right hand side. So this is the opposite hand version of it. Let's go and start creating drawing on it. And this time, I have used my predefined templates. So this will automatically populate the standard views on my sheet. I don't have to do that manually. If you are looking to implement the pre or create the predefined templates for you, feel free to shoot me an email. I will share my email address at the last. So over here, I have my three standard views. If you can three standard views, front, top, and right. And then I will, yeah. Now I'm going to add some dimensions here. So to add the dimensions, to add the annotations, it's as simple. You can use your center marks to place some center marks on the circle. Along with that, you can add the center line. So I'm gonna use my s key shortcut. So press the s key on your keyboard, and you can click on your shortcut keys from there. So I'm using the center line. I also would like to create a center line vertically, so I will select the side edges there. Why I'm trying to show you? Because I I'm pretty sure you guys know about all this, how to add the center lines and all, but I'm trying to show you, okay, you can create the same drawing within few minutes if your model is carrying all the information from the other hand from the opposite hand. Right? Once you've done that, now you have option to add the dimensions in there. So either use the model items or smart dimensions. Using my mouse shortcut key, I'm selecting the center mark and the, center line to give the dimension on the top, on the right, and the distance between both the holes at the bottom. Quickly, I will give the dimension overall dimension on the front view from the top right hand side to the bottom left hand side. Right? And same as for the right view. So this is just for explaining explaining that you can give the dimensions as you wanted. So there is nothing different. You don't have to manipulate your dimensions or change anything. And if you look at your feature tree title block. I'm sorry. If you look at the title block, the name is updated to right hand enclosure. So, again, this information is coming from your model along with the material carbon steel, the part number, the weight, everything is coming from the model. Perfect. Let's go and add a isometric view. So using the predefined, right now my view is aligned with the front view. I can press the control key on my keyboard and easily move your view anywhere on the sheet. So right on the top there and change the display style to shaded with edges and click okay. So my isometric view is there. The next thing I wanna place here is the, flat pattern. Right? So it's a sheet metal component. I have to give all the details for the flat pattern. So as Solvix create the standard views for us, so I'm going to pick the flat pattern view from there. So just drag and drop it on your sheet. Oops. It's too big, so let's rescale it. So click okay, and then you select the model again. Select the drawing view again. And on the left hand side, in the property manager, you can change the scale from one ratio one to one ratio two, and click okay. I would also like to reorient this model, like, upside down. So I will simply go to, the rotate command, and you can enter the radius about what you want to rotate. So one eighty degrees and apply. Perfect. This look exactly the drawing I would like to see. Next thing, I also want to clean my drawing a little bit. So I'm gonna add the bend table in it. So right click on your view, go to tables, and there you can select the bend table. And I'm using the standard template for the bend table as well. So you can see all the information is carried over to my pen table now. I don't have to, like, keep my drawing messy. Next thing, the properties of a sheet metal. So on just one two clicks, I would say you can add the sheet metal properties. So right click annotations and then cut list information. So all the information that was carried over from your left hand component to your right hand, now you can put it on your drawing sheet. So, again, there is no manual changes that you are doing here. Right? So bend tables are same as of the original one. The cut list properties are same from there. You can see the bounding box, length, width, everything is there. Now at the last, I would like to add a note at the bottom saying this is the opposite hand version or right hand version of my enclosure to one zero zero. Right? And then I can just select them to highlight it so that shop floor guys can see that clearly. Okay. This is the opposite hand version without any confusion. So select that and bump it to 18. That's too big. Let's let's change it to 14, I would say. So once you select 14, you can change the color to red and okay. You can make it bold. That's fine. Now as you can see, within few minutes, we have created we have added the standard views with the flat pattern along with the notes, and all the other information is coming from that model. Right? Let's go ahead and save it. So you can save it again in PDM or in your local drives, wherever you would like to. Once you save your data, now let's do a quick comparison between my left hand drawing and the right hand drawing. Right? Okay. So for that, again, I will tile my screen here. So go to Windows, tile vertically. And if you let me clean the screen a little bit, and there you go. So now as you can see, my both patterns, both drawings are completed. So both have the three standard views, isometric flat pattern, along with the note that, the guys can look at to understand, okay, what from where this is coming from. Right? And I'm I I think I've missed the bend lines on the left hand side, so let's quickly add the bend lines there. Perfect. Now my drawing is looking complete here. And yeah. So is again, I would say instead of creating your drawings manually or copying them, making it duplicate, that's not the ideal way. If you are using the mirror commands to create them, the best approach is to create your drawings again because all information is already there in your models. Right? And this ensures the clarity, reduce your errors, and keep your documentation consistent. Perfect. Let's, see what is the takeaway from the today's session. So use middle part for your clean symmetry. Right? You can break the link only when needed. As in my case, in the first two scenarios, I haven't break the link because I want to keep them consistent. But in the sheet metal, I just broke the link because there are chances I have to add more features to it or remove some of them. Right? When sheet metal bearing preserves your flat patterns, that's the best thing. Use the left hand or right hand naming for your clarity. Drive configurations only when manufacturing is identical. And drawing auto update. So why I'm saying drawing auto update? Because if your models are linked or if they are not linked, if you make the changes in the model, your drawings will automatically update and avoid any duplication there. So this workflow saves you 50 to 90% of modeling time. They reduce your errors, improve clarity, and keep your drawing consistent. So I would say opposite hand version don't have to be a headache anymore. Perfect. Let's move to the next one. So as I said initially, the first observer will get a shout out here. So thank you everyone for sharing your guesses in the chat, but winner is only one. And a big shout out for quick observer goes to Nathan Leslie. Sorry if I spell that like, pronounce it wrong, but it's Nathan Leslie. So congratulations for you. Yep. From here, thank you everyone for staying connected until the end of the session. If you are still here, I'll take that as a sign that today, swap through give you a clarity on how to work with the opposite hand parts while maintaining your design intent. And I'll be around. I'm happy to take any questions now if you have. And, before we wrap up, feel free to scan these QR codes above to subscribe our YouTube channel, to subscribe to our technical blogs, and the middle one, middle QR code is for, to register for our upcoming tips and trick sessions. And if you would like to continue learning at your own pace, I would suggest you can simply click on the green check button on the top, to explore our self paced trainings. Thank you very much, and let me see in the q and a tab if there are any answers that I can answer. I can see a lot of questions is already being answered by my colleague here. But, definitely, if anything is missed, I will reach out to you on your email. Or if you have any concern, questions about large assemblies, PDM, predefined templates, anything related to SolidWorks, feel free to reach out to the co engineer technical support team, or you can reach out to myself. Here is my email address. Yep. Thank you very much for connecting. I hope you have learned something new.