SolidWorks Drawings Template Webinar

hello and welcome to our video on SolidWorks drawings and templates this is Carl Schultz one of the friendly handsome and intelligent business consultants here at inter CAD we're gonna be going over quite a few things in this lab in this webinar including custom properties and how to get them on to your drawings immediately without any any extra tricks modifying templates and setting them up and a few bits and bobs is for CAD administration and doing the property tab builder so without further ado we'll get started so the first thing I should mention is that my SolidWorks setup right now should be exactly like yours if you've installed it fresh out of the box so all of the settings all the templates everything should be exactly the same as what you've got if you haven't made any modifications so first things first custom properties what are they custom properties are often called metadata and the same way that in all windows files you have things like date created and date modified you have information about the file so in specific files like JPEGs or mp3s you may have additional information like the artist when it was recorded things like that we can do the same thing in SolidWorks adding things like who the designer was what material it's made out of what it weighs um things like that and have it automatically update those as we change our design or as we as we need it to be different properties and have those automatically come into our our drawings so the way you get to the properties is right up here at the top of the screen there's a little card with a hand on it and when we click that it comes up with this this dialog and so the property names initially with our generic part file we just have this this list that we can pick out bits as to what's important for us so the description the number Finnish there's all kinds of things on this list everything from do not spin author company name division anything you could really imagine and if it's not enough you can actually edit this list which is over in this right-hand corner we just click Edit and now we can actually change things around we can move things up or down in the list we can delete things that we don't like and we can actually add in important new properties that we want to use just by typing them in at the top and then hitting add and then of course we can move them up or down to wherever we need them to be so for the sake of simplicity I'm going to cheat a little bit and link up to a file that I've already created that has a simpler list of file properties in it so one of the themes here is that when we we make these templates these different files that we need for SolidWorks to reference that's great we store them in some safe place and we just need to tell then SolidWorks where to look for these different things so most of these files you can have multiple copies of multiple versions and that's that's no problem the way we point SolidWorks to it as we go up to the top here which I just pressed was the system options and we go to file locations so the first one is always defaulted to document templates and we are going to be modifying that momentarily but for right now I want a different one and of course there's there's lots of different files that SolidWorks uses in this case we want the custom properties file which is right here like I said before most of these files you can have multiple copies of and choose from a list if you have three versions that you like to use one of the exceptions is custom property files you can only have one of these you can see the ad is actually grayed out right now and so what we can do is delete the current one and we can add this in and I've created this this folder here on my desktop for the purpose of this this video custom properties generally you'd want to have that on a network location somewhere where other designers in your company can see it and of course somewhere that's automatically backed up in case of data loss if you if you are using the default directories there's there's nothing actually wrong with that it'll work just fine but if you are unfortunate enough to experience a crash of your hard drive all that work you've put into creating those templates is of course going to be gone so I've I've now relocated to show that custom properties and now when I hit this data card again and I go into list you can see I have a nice simple list of things that we can put into there so we're going to put a few things in here just for simplicity and then we'll move right along to creating the drawing template so the way I advocate doing this sort of thing is to actually create a file with a bunch of the properties that you need that you like and go ahead and then make the template that way that way you can test it you can go back and forth rather than trying to create something actually from scratch is is actually harder it's it's easier to make a dummy model and use that one of the things is you've seen I've just been typing in things here into this value text expression one of the other options is that we can actually link it to things for instance the material and the weight we can link those to this this gobbledygook that comes up SolidWorks understands this what the material actually is specified over in this panel here same thing for weight we can link that to mass and it comes out as 150 point zero zero things after this expression like G so that we know that it's grams and not kilograms or pounds or or anything else and you can of course modify that as well in your document properties you can change the units if you wanted to do kilograms instead of grams for instance you can modify that if you save that into your part template that'll always be set that way and you can see when we go back into our properties here it's now 0.15 and we'll add the K to signify kilograms so I do need to save this part before I can draw it so I'm going to do a save and we'll go ahead and save this just right on top of that that webinar folder here I'll just give it a name and we'll save it so when we hit make drawing from part SolidWorks comes up and it asks us which template we have generally you have these these two templates and tutorial and you can select one if you add more folder locations in that file locations area you'll get more tabs here well we'll do that in a minute so you'll see it and and then you can you can set which ones the defaults as well so if we hit OK next it asks us to select the sheet format sash size and so this is probably the number one thing that new users get confused with and in fact many veteran users are still confused with the difference between these two when it comes to SolidWorks drawing templates there's there's actually two files that control it drawing templates control things like line weight the units the precision and tolerance that are automatically dictated which you can override individually and then the second part is the actual size of the virtual piece of paper the title block and the border with the the letter markings and number markings for a coordinate system is in a second file which the drawing template then references so I'm gonna do a nice and simple a four to start out here and this is again just the the generic one that you see everywhere in in SolidWorks so when we first start out everything's blank if I then drop our part on to the drawing just like anything else it actually fills in some of those properties that we had filled out before so you can see title comes up with degree and so those are already tied SolidWorks has done some of that work for us material the way down here at the bottom and you'll notice that this one called drawing number is actually not a drawing number at all it's actually attached directly to the file name so we may or may not want it to be that way if we are using our file names as the part numbers that'll work just fine if not you would definitely want to modify that so the way actually going I'm going to show you how to actually attach it to put the drawn in name as the engineer and so we go into edit sheet and all we have to do is to add a note so we click note I'm just gonna put it in a generic location and so we could type in you know Carl because that's that's who designed this part and that's fine it works we can change the font of course if we highlight it we can change the font to whatever it needs to be and go ahead and then move that note to wherever it needs to be so that works okay but you're gonna be stuck the the whole point of this exercise is to just just like when we build our model as a part separate to the drawing when we make changes to it all the dimensions are update we're going to be doing the same thing here so that way if we change any of those custom properties say the finish we want to go from a painted finish to something that's anodized it'll automatically update on to our drawing sheet and it's all linked together so that we don't have to worry about it we're essentially making the drawing as dumb as possible to reduce work for ourselves so instead of just typing in my name to this note all we can do is actually of course remove the the writing that's in there already we can click this button over here and you'll see it's got the same symbol as this one up at the top for custom properties except it's got a little piece of chain there saying its linking to property so if you click that button it brings up this dialogue window and what that shows is basically what things you want to link to so current document remains that we're gonna actually link it to the custom properties of this drawing and now that's like not exactly what we want to do because we want to make the drawing almost independent and as dumb as possible so we want to actually do is to link it to the properties that we've set up in the part and so what we do is we click this second checkbox specifying that it's the model viewed specified in sheet properties so when I when I grab this list then it shows the ones that are already in the file properties and this is another reason to actually set up a dumb part with all of your properties already filled out with some generic things because if you have just any part in here you'll always have these SW ones and these are the things that are already like that are already from windows things like file name the folder last save date things like that and you can see these other ones that don't have so much gibberish to them these are the actual file properties that we put in before so I'm gonna select engineer and hit OK and so now of course it says the same thing it says Karl but now that's linked to our file from before the part so if we go back to that part we decide that we need to have last names on all of our engineers just put an initial of Karl s you go back to the drawing and there it is it comes in as Karl s if so that's that's the basic premise so if we go back to edit sheet and we'll go ahead and delete these two drawing views back out of this drawing and if we hit rebuild of course all the things go away the one thing that doesn't go away is of course this name because our actual file name hasn't changed it hasn't gone away but the description and the engineering weight material etc have all disappeared if we go back into edit the sheet we see these other things so this is what actually SolidWorks reads is this PRP sheet means that we're referencing things that are linked to that part so you can see this long one says PRP sheet and June denier and it's it's broken up by several lines and if I try to modify this who got their own notes there so if I try to modify this note I stretch it out and I try to make it fit in that box you can see I can't actually make it go like it was just a minute ago I can't make it shorten itself and so this is another reason to do this with a part actually already in there so if we go in and add in that the same three view that we had before of our part that we just made it brings it back in and when we edit this now we can actually grab this one and move it as we need to changing that box to fit where it's going to fit and of course we can change all the justification settings and and anything else that's a visual issue so again if we go back and delete these views rebuild we can see that going back into the sheet it's this way where we couldn't make it that way before without the part actually being in there one thing to always be cautious of is to know whether you are actually editing the sheet or editing the drawing area another reason to have a part on the screen the parts disappear when you're editing the sheet and of course all these lines turn blue which is a good indicator the other thing I'm going to do is go ahead and insert a picture our logo here at Inter CAD which is stored over here and it comes in very large obviously so shrink that down and they'll put that up and up in this corner here and so there we go we'll even go ahead and draw things in we'll get that actually into the corner and we'll draw some lines in there just to give it a bit of a border and so you could for the sake of time I'm not going to you know modify the the entire the entire sheet but I'll delete just a couple more things here and just so we can see a difference between the generic template that SolidWorks has and the one that we've modified here just for future reference so now what most people will tell you to do is first of course go back to edit sheet otherwise every time you load what's going to be your new template um you'll be in that edit sheet you'll have to right-click - in order to drag views on it's very annoying most people say you just come up to the top now you hit save as and save as a drawing template and that'll work sort of it will load up this sheet format and be okay but you'll see if we actually hit and try to add a second sheet it adds this old one there's there's no inter CAD logo the signatures back and if we were to show it the the engineer would be gone as well and that's because we haven't actually changed the reference to this new sheet format that we've just created so what we actually need to do is go up to file and choose save sheet format and so of course it takes us back to the standard location where all of the sheet formats for SolidWorks are saved and because we're making our own custom ones we're going to go ahead and save it in that that same safe location under sheet format and just call it a for inter CAD we save that one and now under this properties we'll see that it's pointed to of course still the a4 landscape this is the program data it's the one from SolidWorks so if we browse and just do this one extra step and we point it to the sheet format that we just it'll actually have that as part of the drawing template and now when we hit second sheet it comes in you can see everything is is changed with those updates and this is where people really seem to struggle they with not getting changes to stick basically it's it's especially prevalent when you've already created your template it was good but there's some things you wanted to modify some some things you want to improve you make those improvements and for some reason your template isn't showing those additional changes this is the the number one reason as to why that would be happening is just not saving that sheet format and giving it a reference so now we'll actually go ahead and save as just like we're gonna do before we'll actually save this drawing template now that we've got it again it as soon as you change the file type to drawing template it takes you back to the SolidWorks default locations and we'll go ahead and change it to our spot here under document templates and we'll call this inter CAD part oh if you don't click in the box first inter CAD part click Save and okay so then it comes up with this warning says templates stored only predefined in empty views so models dimensions etc will be removed basically what this is saying is that if you've got other stuff in there like I said the best way is to load this with a part already in it in this case I've deleted it back out it's warning us that those are going to show up empty all the annotations and things like that'll be gone you can if you choose save something like a three three standard layout and then when you hit make drawing from part it'll actually go through and make those fill in those three blank drawing views for you and of course that is saved to the template not to the sheet format again just to repeat the sheet format covers the title block the order and these abc123 the border whereas the drawing template is things like the drawing views the line weights the dimensions the the things that would be covered in a drawing standard so we've got two saved it it's of course the the drawing number we didn't change this so now it says inter cad part because that's the the new file name and we can just close that that'll be that'll be fine so if i go back to our our generic part that we created earlier and i click make drawing from part well there's all we have is the SolidWorks ones and the reason for that is we haven't we've we've created these new files but we haven't told SolidWorks where to look for them so again we need to go to options go to file locations and this time we can just add in these new locations so it's document templates we also want to change this one and go to the sheet format which is right here and we want to add in our new area for sheet format one thing to keep in mind is if you want this to be a little bit cleaner you can delete these corporate ones from SolidWorks the ones that are pre-installed you can delete those back out and then you just have your basically the ones for your company the ones that you've modified and and are approved initially I don't recommend doing that just because if you mess up your templates or something goes awry it's just a little bit of a pain to get back in and find this this long extension of SolidWorks program data todrick's 2013 laying english etc just make sure you keep it for long enough that your content and happy with the way your templates are working before you go ahead and delete those back out so with those new ones added in I'm not going to add the search path we can do make drawing from part and you can see up at the top here now we have a third tab and we have the inter CAD part drawing or the inter cat drawing I should say and of course it's it's set for a four so one thing you'll notice is that when we started our template basically it automatically jumped into a four whereas when we were using a SolidWorks one it actually asked us which sheet format we'd like to select so the way that you do that what I'm going to do is actually just have a few that are already set up so I'm going to take these finished ones here out of the oven and just move some files around along so we'll delete the old ones and we'll put in these ones that have already been completed so I have two here for sheet formats one is a two and one is a four and we will delete that one and we'll keep that one in the oven for now so and we'll actually go ahead and and open up a second part here so this again this is a a part that I've already created and you can see if I click on custom properties it's got a bunch of things already filled out so if I click file make drawing from Part I click enter CAD metric again it just pops through so I've actually modified this one so it's it's just a little bit more finished and all these things come in nice and pretty with the approvals the the drawn by the finishes the title etc but again it didn't ask us for what sheet format we'd like it automatically selected this a4 so the way we get around this is we have two resave our template so the drawing template if we actually delete the sheet format and then save and then save our drawing virus excuse me our template again it defaults back to this location you want to make sure you go back to your save location so we're just going to save right over this inter cad metric right into it so do you want to replace it yes I do it gives me the same warning about priest priest stored views and annotations etc and now it's in there so if I do the same thing I hit make drawing from part I choose inner CAD metric hit okay just a bit of a technical difficulty there when I had saved that the first time I didn't delete that sheet format I've actually fixed it now so if we go make drawing from part go to inner CAD metric it actually pulls up this list and this is because I've got all of the possible sheet formats I also have will show that actually so if I go to my file locations I've got four sheet formats I've got two bits in here one is the the corporate program data one and one is on my desktop here under webinar so I've got the two that I put in there out of the oven and I've got the whole bunch from SolidWorks so if I actually remove those locations from sheet formats I'll just go ahead and remove the default ones hit OK now when I hit file make drawing from part I select my template that has this template now has no sheet format assigned I've deleted it and then resaved the template hit OK now it only looks in the area that I've selected which is in my webinar folder of just those sheet formats and I can choose a two or a for for the the following file I can also do that again so it loads the previous one and I can change that to a two for the next or a four for the next one and have a smaller one so the the last thing I want to cover in in this video is the property tab builder so one of the the files that one of the issues that I've run into in previous companies is what can happen is with things like engineer just for a quality standpoint sometimes you'll type in K dot Schultz sometimes you'll type in KS different designers like to like to put their initials in or their first name last name etc and to get away from this what you can do is use this property tab builder so when you first hit it of course it has nothing in there we haven't created this one and so I'll just go ahead and start a simple one so we start the the tab builder and it comes up with this one just FYI have the way to get into this property tab builder you go to all programs SolidWorks 2013 SolidWorks tools there's a number of things in here that are very very useful in this case the property tab builder is the one that we're using so it's it's a pretty simple interface it's just kind of a a drag-and-drop so we can do text box we can do lists and so what we want to do is is add a caption so that we know what this is engineer we want to link that to of course the property that matters which is engineer and then we can type in specific values for for our engineers or designers and this then makes it a little bit more limiting it doesn't stop somebody from coming in and coming in directly through this this way and actually typing in but it does make it easier for them to use the right appropriate thing that you have to go through and do it manually to be a bit of a pain for you so I'll just put in one more here change that one to description and we'll leave it blank for someone to fill in so we save this and there are different templates for this property tab builder there's one for parts assemblies and drawings this one is obviously just for a part and you store it in the same location as that custom properties file the properties dot txt so I'll do this one as live and I'll save it and now if I start a new part new part we pull that up and so if we choose from our list we choose mr. Haly and we choose a description of computer buttons because they're right in front of me if we hit apply you can see that in this custom properties area they've already been filled in for us so if you build that up to kind of a full document again I'm going to steal this one out of the oven we'll delete the one we just made and replace it with template there we go so and here it is so this is the things that we're already on this part obviously so when we're looking at this we can then change all these two different pieces change the dates so this was a drop-down that I created that's only a calendar for drawn by approved by and we can actually the material actually pulls from our same list that would be over on our part very handy and you can actually use this to apply things like engineer to multiple parts at once saving you a bit of time so you just basically but they don't reset the fields from one part to another so if I start a new part you can hit apply open the next part hit apply hit apply it apply and update all the the properties at once just so that there's no errors typos it's just an elimination tool so the last thing that I want to go over is so we've we've got our system all set up we we have all of our file locations set where we would like them everything else and that's great we've got everything looking how we wanted to problem is the guy sitting next to me hasn't been messing with this for the past two days and all his stuff doesn't point to the right place so we could go through and go you know item by item changing those file locations the same way we did on our computer or we can actually use another one of these tools that are buried in the Start menu called the copy settings wizard this is very useful in general for a number of different things if we hit next and this this gives me a warning here basically you shouldn't be running SolidWorks when you run the copy setting wizard and I'm just going to go ahead and ignore that offer that warning so we can use this to save out all of the customization that we do to SolidWorks again if you are unfortunate if to have a hard drive crash if you do a lot of things with shortcuts with changing where the default locations are for the toolbars and of course things like these file locations and and your settings you're gonna lose that so this is another way to safeguard that so we can save all of our things because this is my personal file that I want to return to later alternatively we can turn off all of these other bits and just change just save those system options and we could then save this file as inter CAD SolidWorks settings hit next and it will actually save just those system-level options we put that in a safe network location again some somewhere that's a bit redundant and then all we have to do is get the other users to hit restore and then use that to pick up their options very useful and it'll only restore the parts that are saved if that makes sense so if you only saved the system options that's all that will get restored so you can have them save everything of theirs and and do a mix and match for different files like this so that's all I have for the the practical demonstration so the what's next I've I've blasted through quite a bit of information here in a short amount of time this is the sort of thing that is covered in our drawings trainings at Inter CAD we have a few of these courses coming up these are obviously for 2013 after the essentials course which is our intro level course to get you familiar with SolidWorks drawings training is the one that I recommend the most and the reason for that is as a designer myself I love to design it's it's what I live for and drawings is awful anything that makes it so that I can do my drawings faster and easier is is what I what I strive to do and that's what this course is about it allows people to just be faster spend more time doing design developing new products getting those orders out the door so I highly recommend them if you're interested in taking our drawings course they cover obviously much more than just these templates they cover things like the dimension expert and bringing in almost fully automating nearly your drawing so that you can actually do all those mark everything inside the model and it just comes out directly on that drawing almost automatically so if you'd like to sign up for the drawing courses you can of course contact your local business consultant here at inter CAD one thing to note here is that I'm actually leaving inter CAD as of February 15th in the interim please contact Allen wicket he can be contacted obviously the the emails are pretty straightforward it'd be allen wicked at inter cad comm a you with that thank you for watching this whole video I know it's a bit dry in a bit long but hopefully I give you a bit of of information helped out a bit and hope to see you at our our next event or our next webinar thank you

Channel: Karl Schultz

Views: 25,867

Keywords: SolidWorks (Software), Computer Aided Design (File Format Genre)

Id: x1KonvhwNg4

Length: 36min 42sec (2202 seconds)

Published: Mon Jun 02 2014