Transcript for "Clean Up Your SOLIDWORKS Drawings: Dimensioning Tips & Tricks":
Hello, everyone. I am Michael Dady, senior applications engineer at GoEngineer. And today, we are going to be reviewing how you can improve your SOLIDWORKS drawings. To do this, we're gonna start out with some well known items, some of which have some new Oryx. Then we'll see some up and coming updates from recent years. And finally, we'll talk about how the three d experience platform can help your team communicate. Alright. So let's take a look at the well known items that most of you may have seen before inside SOLIDWORKS. And anytime we Artec talking about SolidWorks drawings and I'm giving tips and tricks or ways that you can help save time with SolidWorks, I always start with this topic of model items and smart dimensions. No, why do I talk about these items? Because I believe model items is the single biggest time saver for drawings that you can use. The reason being is most SOLIDWORKS drawings reference a part model or an assembly model that has feature dimensions, sketch dimensions, and other items that we can use. If those dimensions happen to match, or annotations for that matter, happen to match what you need for product manufacturing information, model items is a great tool to import that information into the drawing so that you don't have to repeat work. When we do so, we can import dimensions, annotations, reference geometry if we want to. We've always been able to eliminate duplicates with dimensions. More recent update to this has been eliminating duplicates with notes and other annotations. When we do this, we can we have multiple ways that we can add the information to the model. We can choose a selected feature and then import it into a specific view if we have a pretty complicated model and we only wanna show certain information, or we can do the entire approach and do the entire model and use all the views. You can pick and choose what information you add to the drawing when you're doing this. And, again, we can use instance counts for dimensions, whole callouts if we want to, whole locations, even hole profiles from hole wizard holes. When we do add the information to the model, you can see it quickly No only adds our dimensions to the model, but it also organizes them in a Zeiss, neat way, centers the dimensions. These two here, which would have overlapped each other, they automatically move it. So it brings you in a nice, clean, neat format for this process. If you happen to delete dimensions now these are just removing the dimensions from the drawing. They're not deleting them from the Metal, but it will also reorganize the dimensions for you. So it's a nice quick way to quickly add a whole bunch of information to it. And then after you're done adding the model items, you can go ahead and use the smart dimension command to finish up any of that to add any information that's not included OrCAD add other annotations as needed. Now these dimensions that are organized nice and neatly, they are using the document properties for dimensions. Now before I talk about those settings, I do wanna make a note of the document properties. Every company usually has their standard templates that they wanna add and have the company use. However, as new updates come with the software, as your company changes their policies with how you wanna do CAD, you know, convey your information and settings inside the drawing, those things will change. So when you go and work on an older drawing, now everything's been changed out. And that's when I wanna mention the save to an external file and load from external file. So you can take those new drawing settings or if you guys have CAD admins who take care of this for you, they'll they can possibly provide them. So you can save your new settings out to an external file, open up an old drawing, and then load those new settings. And now your drawing is all added and it's up to standard and set up the way that you want it. When we're talking about dimensions, the way that those dimensions were laid out on the screen, it's the dimension settings for the offset distances, also for extension lines, radial leader snap angles and things like that. But I wanted to talk about a couple of new options. Center between extension lines, that's a nice option for that's why our dimensions are getting placed in there nice and neat. Also, a new item that's recent as well is highlight overridden dimensions in a different color. So anytime we use the smart dimension command to add a dimension to our drawing wrong one. Don't blame the software for the guy doing the picks and clicks. We can add a dimension. This is a driven DyeMansion, whereas when the model changes, this dimension will change as the model does. You can go in and override dimensions in this case. I tell all of my SOLIDWORKS essentials students, don't do this because it will break the parametrics that are in the model. But some companies will do that. And when you do change the model the the overridden value, you can see that the color has changed so that you can clearly see this dimension has been overridden. So that's a new feature. Now you're probably saying right now, okay, Michael. Why isn't everybody using model items? There's a couple of reasons. Some companies don't like model items in the drawings because model items dimensions are driving dimensions. So if I click on this dimension, I can go in and I can modify the model directly from the drawing. And some companies don't like the fact that detailers can do that. The problem I have with that argument is you can't do it by accident. Because you can't you don't have instant three d that you can just click on a dimension and accidentally type in a number. You have to double click on the dimension, modify the DyeMansion, and then hit okay and rebuild the model. So the chance of somebody doing this by accident are very slim. So if you have a diligent team, this stuff you can it shouldn't be a problem to let these items in there because it is a huge as I mentioned, it's a huge time saver. Alright. Let's take a look at other ways we can save some time as well. Another way that you can add dimensions to a drawing is with with feature dimensions is through the use of annotation views. Anytime we create a feature and add dimensions to it, they those dimensions get assigned to an what are called annotation views dependent upon the orientation of how you built the feature. They're inserted automatically by the software, but you can also insert your own annotation views based on an existing direction or you can select a direction. And then when we do that, you can actually move annotations from one annotation view to another for downstream use. The way that we can use these annotations is when we make a drawing from a new model or from a model. And if we go into our view palette, you can see that the view palette, we can import annotations and we can choose design annotations. As we drag and drop these items in Creaform my top view and our other associated projected views, the dimensions that are the feature and sketch dimensions that are associated with those view annotation views with that orientation will automatically be added. The same thing is true if we use the model item model view command. We can choose to add those annotations in that property manager as well. Unfortunately, unlike model items, these are not organized nice and neat. They drop them in there. It's not nice and neat. A lot of people are familiar with No these items and dragging them one at a time. The dimension palette, which is a great tool to save time for adding properties to a dimension rather than using the property manager on the left. But you can also select all your dimensions in a drawing and use the dimension palette. And on the bottom, we have a variety of different items that we can arrange. So auto arrange dimensions is the one that I'm gonna use. And when we click on it, you can see all our dimension snaps and everything are set up. Our set up for in the using the same snap lines that we used before. We can still delete the dimensions out of the drawing and not use them any longer, but you can there. So you can see it adds time, and the dimension palette can quickly rearrange these dimensions. Another way we can save time with, working on dimensions and adding dimensions, you can see that I have a dimension here, that has a plus or minus tenth out tolerance on it. And we can take that tolerance, and we can use the format painter to quickly add those dimension settings to other dimensions in our model or in our drawing. Sorry. And then we can quickly add them to whichever ones we want. Another great way to add change dimensions is through the use of styles. Styles, when you initially create them, you can add a you modify a dimension, change it the way you want, make add dimension text to it, and then you can add a style to it. Then we can take and go to another dimension that we wanna apply the same style to, and it will automatically update that dimension to match the new style. We can also save out the styles and load them if we need to. So if you have so right now that style is only stored in this drawing. Actually, it's actually stored in the model, but you can access them in the drawing since that's some design annotation. You CAM so you can save them out and then load them in a different drawing so that you can update with other so that you can update and use them in different locations. Alright. So we can quickly reuse annotations from the model in our drawings, saving time. The dimension palette allows us to rearrange dimensions quickly. If we want to duplicate dimension settings, we have the format, painter, and styles. And finally, annotation views can be used to organize dimensions. So those are our tried and true methods. Let's take a look at some of the new changes that we have available. Okay. We've always been able to, a great this is a great tool for clutter. We've always been able to use dimension break lines. Kinda there we go. So we can add dimension break lines, and we've always been able to use them so that we can see where leader lines cross other DyeMansion. New in 2026, we now have the ability to add break lines to dimensions, and they will break around text now as well. And not only does it break around text, it will automatically update as we move these items around. If we happen to add a dimension and it overlaps an existing dimension that we have a break line on, we can either right mouse click and add a break line, or we can right mouse click and just update it so that it breaks around the text. Very easy and make sure that we clearly see what information is being conveyed. Another new addition in 2026 is existing technology that has been updated. We've always been able to use magnetic lines to reorganize balloons along with drawing views. But now in 2026, we are able to add notes, other different notes, weld symbols, and a variety of other annotations to magnetic lines. We can drag them on there, or we can use the MODSIM magnetic line command and collect them as we're creating the line. We can also quickly add other dimensions to an existing magnetic line to organize them as well. So lots of new options for that. The next item that I'm gonna talk about is not anything new, but it is new for drawings. We've always been able to save, always been able to reload the SOLIDWORKS models, both assembly and part MODSIM, if if we needed to. Let's say you go in and make a bunch of changes and decide, you know what? This is all I was foolish. I shouldn't have gone down this path. So same thing with drawings now, and you CAD always reload. You can do the same thing with drawings, Do a quick reload command, and it will warn you about it. And then you can quickly go back to your last saved version on a drawing. Again, more of a time saver than an uncluttering the drawings. Alright. So our next enhancement is an improvement on an existing item. We've always been able to do baseline chain dimensions and ordinate dimensions, but there has been an improvement recently to chain dimensions that when you are using them, it will do everything it can to maintain maintain collinearity of those chain dimensions as you're creating them. It will automatically there's a setting now that will automatically under our document properties, dimensions linear, we have added options for chain dimensions to offset text automatically when space is limited and also to change the arrowheads when they're overlapping each other with some very tiny Dady. So we can add those items too. Also, we are able to add an overall dimension to the entirety of it. And as always, we can switch switch between chain and baseline dimensions as well. Alright. Our next item is something that, most users will already have. I have a model here. I am connected to the three d experience platform through the add in. And when you are inside SOLIDWORKS desktop, as I mentioned, most of you probably already have this technology available to you, since for about the last three years now. Any new license of SOLIDWORKS has had cloud services attached to it. And with cloud services, when you are attached to your tenant, you can go in and automatically generate drawings based on your system settings that I'll talk about in just a second. You can do multiple multiple models at once, and it will use your default system options OrCAD drawing Ortems for a drawing template, for BOM templates, and rev tables. And what it will do is create a new drawing of this model. It'll interrogate the model, go through and check it out, see what's going on, and then it will eventually using these settings for default templates for your drawing and your file locations for, both BOM templates and revision tables need to be taken need to be set. And what it will do is it takes that model, automatically creates a drawing with your default template, and adds a rev table, BOM table if there's an assembly as well, and it creates what views automatically. Now this is a beta Success. This is a beta beta version of the software. Sometimes you'll get dimensions that aren't usable, but you can clean this up and quickly use the other tools we've talked about earlier to create these items for you. Alright. So dimension break lines have always allowed us to clearly see what features are dimensioned, and and they have even gotten better now that we can break around dimension text. We can neatly organize a variety of annotations with magnetic lines. Drawing changes can now quickly PBI undone with the reload command. Chain dimensions are even more powerful with new Oqton, and drawing creation can be streamlined to remove repetitive tasks with the power of the three d experience platform. Alright. Let's talk about collaboration. When in the when the typical paradigm that we've been used to at when we're communicating information downstream is pretty much been the same. If the downstream user, whether they're internal or external, we go in. If they're a if they happen to have SOLIDWORKS, we go in, we do a file pack and go, and then we email the person Oryx we upload it to a cloud site and have them down you know, we can send them a link and have them download it. A variety of different things, you know, is but it's manual. We can also if if they don't have SOLIDWORKS, now we're talking about they have to have PDF or we need to do a DXF, a DWG, or a STEP file depending upon what we're sending them. But it's still very much a manual process. And on top of that, they have to have the software that you can that can read this. Edrawings has been one way that we can access SOLIDWORKS models and and send drawings as well, DXF, DWG files. But, again, it's another piece of software. So as I mentioned, most of you already have access to the life cycle and collaboration. You you already have access to the platform, and you can share your files through the three d experience platform out there. So let me do some quick rearranging here, and we're gonna learn a little bit about how that process works. Sharing your designs and getting feedback from anyone just CATI easier with SOLIDWORKS and cloud services. So let's see how to do it. With any file open, go to the life cycle and collaboration tab. Now under share a file, first click on the arrow to verify which file format you'd like to share. Three d XML is the lightweight format for short load times while maintaining exact three d geometry. Once you click the share button, the file is generated and uploaded to your three d drive in a folder named share with external. Now we can copy the link to that document if we want to grant wide open access. Most of the time, though, I want to make use of the two options below that. Slide the first toggle to let anyone add their comments and see anyone else's comments. Use the next option if you want to restrict access to specific people. Just add the emails and a custom message and click share. The great part here is you can share this file with anybody. They don't have to have SOLIDWORKS or licenses to three d experience. Now if they're not familiar with the process, you may want to tell them what to expect. They'll get an email like this one with the link. And if needed, they can create the free three d experience account to log in. The file will then open in their browser for viewing and comments. The view mode tool lets them change the look of the model, including the toggle for perspective. Since this is an assembly model, the explode tool is available to automatically separate the parts and visualize how they come together. They can use the measure tool and even mark the dimensions with special flags for instantly visible comments. With a combination of annotations and text, they can mark up the design the rest of the way. The markups are viewable in the view orientation where they're created. So as you move around the model, it keeps it clear of clutter. When they're done, they need to click on share as comment, and that captures all of their markups and makes them visible for you and others with access. That's all they need to do. There's no emails or zip files required. Now back in SolidWorks, you'll get a notification in the my session. Clicking on that will take you to the shared file in three d DriveWorks then click on the information button to get to the comments. When you click on the thumbnail, the three d play app opens right in the task pane for you. The best way to look at all the comments is to use the annotation tours since that lets you cycle through all the views where the markets were created. Going back to comments, lets you reply or add comments of your own, and everyone with access to the link will get the updates. Now you can interact with the shared file in all the same ways with measurements and annotations and text. Just share your own markup as a comment for everyone to see. If the file you have open is a part file, notice you have the option to use the SLDPRT format. This is important because whatever file you share can be downloaded. So if you want them to have access to your SOLIDWORKS files, great. That's an easy way to send it. If you need to protect your design details, consider three d XML. And if you're sharing a SOLIDWORKS drawing file, format options include DXF and DWG. Alright. So it's very simple to use the software. It's right there inside of the design using the three d experience Creaform. MakerBot sharing collaboration nice and easy. Cameo on now. It doesn't require any new installations for software. And, again, the greatest part, you are likely already have access to this tool. Once again, I'm Michael Dady, and I really enjoyed helping you clean up your SOLIDWORKS drawings. We will go through and answer the CAM and a questions Let's see. 2026 was break lines and annotations on Magic lines. Reload drawings was twenty twenty five. Collinear and chain dimensions are twenty twenty four, and AI generated drawings is twenty twenty six as well. I think whole callouts will come out if you include the thread inside of, the staff. Is there a way to quickly display the thread on the threaded stud like there is on a threaded hole? That you should be able to, I think let me take a look at model items real quick. Is there a thread callouts option? Yep. So that's cosmetic threads, though. I don't know if it's possible to do the thread studs. That is something we would have to check on and get and add to this. So geometric tolerances, if you put a geometric tolerance into the model as an annotation, it will come in. If you use DimXpert, you can get those loaded in the same way that you did, that you do design annotations. There's a there's a click right below it that has, from the view palette. I'll actually share my screen here in just a second. So this model has DimXpert dimensions in it as you can see here. So if I create a drawing with it No. I do not want to make a new one. And when we go to the view pilot, there's an option for DimXpert annotations. DimXpert annotations are used a lot for MBD, but they can also be used for areas in the model if you want the model to be the driving one source of truth. You can put the DimXpert annotations where, your product manufacturing information isn't contained in the feature and sketch dimensions. And then when you drag in, You can add so I can go into if I go back to my model and, of course, my control tab isn't wrong. It's not working because I was in a command. If alright. I'll shut off my DimXpert annotations. Hopefully, it'll stay that way. I can go into, tools, ins where's the annotations? There's an insert. Yeah. Insert annotations, geometric tolerance, and I can assign it to something on the model, whether it's a face or a dimension or anything like that. And those geometric tolerances are what comes in with the model items. The expert annotations are a completely different annotation. Yeah. Dim expert annotations are Dim expert annotations rather than rather than model items. They won't the gym dim expert won't come in unless you use the method I showed. Okay. So the other thing that you can do to address that is you can change you can if you take a look at my model dimension, you can change the dimensions in the model as well just like you can inside a drawing. So if you wanna just if you wanna do it, you CAM either do it in the in in in the model and then just use model items, or you can do a driven dimension and add it that and do it that way. But even if you add it into the into like, if I go back into the my print here, that is close this one. And No if I if I add those design annotations again make sure it no. Boom. So if I shut off once it loads, I'll shut off DimXpert, and let's say I grab my top and stuff. You can still now if they're restricted, but you can still go in here and modify this to whatever you want it to be. Alright? And then if I go back to the Metal, you grab my whole pattern, you can see it's changed here as well. do not know the so is there a way to show cosmetic threads with visual setting as hidden? I do not believe so. If the thread is hidden what the visual setting is hidden, I don't think it will come into the drawing clean if it's not in the model clean. Okay. I think we've answered everything. I think we can wrap this up. Thank you, everybody. Have a great day, and thanks for joining us.