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CATIA Setup, Parametric Boss and Two-Way and Four-Way Locators
A free lesson from Skill-Lync's Automotive Lighting Design using CATIA V5 course, on Grow by Skill-Lync · Last updated 16 Nov 2026 · Session: “2.0 - Basic of Lighting & Software overview Part 2 Seg 1”
What will you learn in this free Automotive Lighting Design using CATIA V5 lesson?
The instructor sets CATIA V5 options and shortcuts, then builds a plastic locator boss in Part Design with draft, fillets and chamfers. The lesson links the model to parameters, formulas and an Excel design table, and models a two-way and a four-way locator that keep at least a 0.5 gap.
- CATIA option settings and custom shortcut keys
- Boss with draft, fillet and chamfer features
- Linking dimensions through formulas and a design table
- Modelling two-way and four-way plastic locators
What comes after lesson 2?
The next free lesson is lesson 3, “Lamp Regulations (ECE R Series) and Master Product Structure” (87 min). Later in Skill-Lync's Automotive Lighting Design using CATIA V5 course (paid): lesson 4, Basic of regulation & start of making Lamp Part 1 Seg 1; lesson 5, Basic of regulation & start of making Lamp Part 2 Seg 1; lesson 6, Basic of regulation & start of making Lamp Part 3 Seg 1. The full course has 12 lessons (21 h 37 min of video); see the course overview or its price and syllabus.
Lesson transcript
Machine transcript of the lesson audio (lightly cleaned). Technical terms may contain errors; the video is the reference.
Part 1
Hi guys. In this session, we're going to start the main tool, CATIA. We are going to use CATIA V5 as a first tool to create the models. So I'll give you some basic instruction, a theory part of CATIA and then we will head over to the actual CATIA. So basic modeling, what are the workbench we have? Some basic commands. So in the mechanical design, we are mainly used the part design, sheet metal design, surfacing, moid, structure design for the production and the manufacturing. However, for the lighting industry, sheet metal design and the structure design is not at all required. So let's, I'll show you some image first, then we will head over to the actual CATIA.
This will be my workbench. As a course requirement, you should be aware about the basics of the CATIA. So you might be knowing these things, but it's my responsibility to give you a basic overview how this CATIA workbench works. And what are the workbench we required to generate 3D model for the lighting divisions. So in the mechanical design, we have part design, assembly design, sketches, product function, tolerancing and annotation, weight design, mold tooling design, structure design, 2D layouts for 3D design, drafting, composite, grid design, core and cavity, healing assessment, functional molding, functional molded, sheet metal design, sheet metal production, composite design, wire frame and surface design, generative sheet metal design, and again the tolerancing and the annotations. So more than 75 workbench are available in the CATIA itself. But we are not going to use those 75 workbench.
We will use first as a part design as initial workbench, then GSD generative surface design, that will be our second workbench, assembly design, and the drafting. This four workbench will do our work. However, if you are into the tooling field or the plastic mold design company, you should learn the mold tooling design workbench. If you are in sheet metal design workbench. If you are in sheet metal design workbench, then you should learn the sheet metal design workbench. Having another knowledge about any of the other workbench will add on to you, but this is the prime workbench you should be aware about.
Generative shape design helps us to design in advanced surfacing based on the combining of wire frame and extensive multipole surfaces features. We will do practical sessions on this, but this is a theory part, so you should be aware. In the surface modeling, we have free style sketch dresser, image and shape, digitized shape editor, generative shape design, ICM shape design, error expert. So these are the workbench mainly used for generating the surfaces. However, in the mechanical design, we use the mechanical parts workbench, like part design, assembly design.
You can see these are the solid parts making workbench and shape design. You will find more on surface design workbenches. So these are the details of the workbench. Let's jump to the criteria directly and I will show you in this session some quick settings and quick shortcuts which you should do. Do before starting the modeling. Okay. As a basic, we should be aware how the CATIA get started and what are the alternative options are available to turn on the CATIA. One, you will directly click on this and it will start the CATIA. This is one thing. Second, if I turn to the run command, I need to type NC next. This will also start my CATIA.
Third way is to go to the menu bar and type CATIA and here you will get an open command. So these are the possible ways to start the CATIA. Now, let's do a quick settings. As a starting point, you will get this workbench. This is a product structure workbench. Okay. So we need to change it. First, we will close whatever has opened. Now, I will just do a quick settings. Go to the tools option. First thing first, you need to click on this data saving no automatic backup.
Why? Because if you do this automatic backup every 30 minutes, what it will does, it will create an automatic backup in your RAM. So your system will get slowed down. Because we are going to make a huge part RAM. So the memory should be free. So you have to check this button on. Coming to the next in the PCS. This is number of undo. So personally, I suggest this should be not more but at least 40. Why 40? Because this will allow you to 40 times do undo.
Mostly what happens in V works on the surfacing. So you have to click undo sometimes. So if you click on 10 times, then you will get only 10 times undo, which is most of the time it will not work for the lighting. So you should be make it 40. Now next display. Now next display. In display, there is a performance. In performance, you have to make this proportional accuracy 0.01. What happens is if you increase this, you can see here your shading will be increased. This will help you to have software more fast. But this will also eat the visibility. So we will vent as low as down. So 0.01. For 2D accuracy also, we have to do the same. Rest of things just keep it like that.
In visualization, if you wanted to change the color of the background, you can change it from here. Black or white, whatever you want. But normally this color is good enough to work with. Next thing you have to check this surface boundaries on with this color and with the 0.13 mm thickness. What happens is if you working on surface and if you got open boundary, then it will be not visible to you if you not check this boundary on. So make sure you will check this boundary on.
Now catch activation. This work with catch system. This should be activated. For huge assembly things, you should be click on optimize CGS large assembly visualization. But currently we are working on single single part. So we are not check this on. Now in infrastructure. Now in infrastructure, go to the part infrastructure. Here just go to the part documentation. In your case, if this is enabled, just uncheck it and make it disable. Suppose this is your condition. Just uncheck it. Make sure your hybrid mode will be disabled. Click on the parameters and relations. This will help you to show parameters and relation in the 3D.
In the drafting. In the drafting, just turn on the manipulators which you think is required. I will explain what are the dimension manipulators you needed. But as of now, just check this 2 on and this one. And this also. So. So. In the compatibility DXF, just turn the MM on and in the step tab, just make it 242-ED1. If you do not have this 242-ED1, whatever the last drop down menu option you have, just click that on. And in the IGS, just turn this representation mode solid shell.
Click OK. Now, my settings has been done. I will move to the Shortcuts now. I will click on New, OK. As of now, I will not give any name, just click OK. Now right click here, go to the Customize. Select the workbench which you wanted to work on. I have chosen Part Design and Shape Design. Just make sure you will select the right workbench that is Generative Shape Design. Here, in the Accelerator, you can define the Shortcuts also. Because, during the designing, we have to switch from Part to Shape and Shape to Part.
So, better to have a Shortcut. So, we are defining the Shortcuts here. Now, I am going to the Command. Click on All Command. Click only one time H. Search. Find Hide and Show. This is. This is my Hide and Show. Not Hide All. This is Hide and Show. Show Property. Define your Space as a Shortcut. Because, this will help us to create the model faster. So, I am defining one Shortcut here. You can choose your own custom Shortcut. I recommend to choose Space because it will help you more.
In the same fashion, so it is saying Space is already used by IMA modification. So we need to check whether IMA is having a Shortcut of Space or not. We will delete that Shortcut and create our own here. Okay. This has been defined by the Katia itself. So we cannot change. So I will give another Shortcut. If you are facing the same issue, just follow the instruction. I will give Control-1. Now it has taken. So Control-1 will be my Shortcut for Hide and Show. I will now check for the Split command.
I will see if it is there. Okay. Split is not showing here because we are not into the surfacing. I assist to surfacing. Then I will try to find that again. Here. Show Property. So this is not, this creates a Split and this is my Split cut down. So I will create a Shortcut Alt plus S. I will check whether it is defined or not for the other. No, it is not defined. Then I can select this one. You can create your own Shortcuts. I am showing you the way how you can do it.
One more Shortcut I would like to add here, Fit and All. This is Alt A. Okay. Just close this. Now we have ready for our Modeling. In the next session, we are going to practice some basic Models. 2 3 4 5 5
Part 2
Hi guys, as in last session, we learned about the settings and the shortcuts. In this session, we're going to head over to actual practice. So this will be going to fun for you guys. And if you are regular user of CATIA, then it will be very easy for you. But if you are used before and had too much time to use the CATIA, then this is a kind of test for you. So you will be familiar with the commands and other things. So you can recall those memories. So let's begin. In this session, we're going to make this type of locator. This we call it as a boss. And this is a 2-way and 4-way locator. So we're going to make this in the 3D modeling. We will try to maintain this dimension and make the 3D model. We will try to make parametric modeling.
I will show you what parametric modeling is and how we can maintain the relations. So let's jump to the CATIA. So guys, my CATIA is opened. And let's begin with the scratch. I will go to the patch. I will go to the part. Give a name, boss. Click OK. I will hide this XYZ plane. I will create my own XYZ plane. Why? Because in parametric modeling, if we use this plane, then we are unable to move our 3D model. I will explain in the end why I have chosen this one. OK. Just make a point at 000 condition and make a new axis on this. Just make sure you click on the point. Otherwise, the parent will not get linked.
How I opened this? Just right click. Parent and children. So there is a shortcut. Right click A. You can find there is a link. So if so, if I move this to 5, my axis will also get moved. Okay. As of now, I am taking it as 0. Just make sure whenever you are doing any modeling, because whatever you do at the first, it will become your habit. So make sure you will check this one also. That is a manual updating. What happens here is if I click on 15, it will not get updated.
I have to click on the update. I have to click on the update button. This will help me to do undo or some mistakes. Alright. Now, I will go next in positional sketching. In positional sketching, I am choosing YZ plane and origin type is projected point. And I will click on the given point. Hit OK. OK. Now, at the background, I can see some kind of grid. I don't want that grid. So I just turn this grid off. If I make any line, you can see there is a point moving at certain distance. 70, 80, 60. I don't want that one. So I just click on uncheck this one.
Now, I can move anywhere. OK. Now, as a basic thickness, I will check this rectangle again. Give some dimension. For practice purpose, I am taking 50 mm. Exit from the sketching. Just make sure, guys, you will not do any modeling in this part body. Every time whenever you have to do any solid modeling, you have to add another body. Go to the solid. How I switched? I created the shortcut. Check out the session one. Now, I will click on the paired command. Select the sketch. I am taking base thickness as 2. If you don't know, remember the sketch model. Just go before and make a sketch in your book.
So, this is my base thickness. This is a T. So, in the given sketch, there is a T. So, I have defined T as a 2. Now, I will create. So, whenever you are selecting the sketch again, just make sure you add another body. Click on the positional sketch. Why is it? Click on projection point. Hit OK. Now, I will draw a circle. Just make sure that you will check this on. So, you don't need to, I will show you what happens when you check that.
It is automatically giving the dimension. If you unchecked it, what happens is, you have to define the dimension. It's again a clicking process. So, to avoid that, you can check this one on. Now, as a D. For D, I am defining the 3. This is my 2D. And the height, I have chosen 2 as a base thickness. I will multiply by 3. So, multiply by 4. Sorry. Because this, I have created on this base thickness on the bottom side. Alright. Now, I will add this body to body 2. Why I have added? Because, when I cut down the section, it should look like similar to my section, which I have shown before starting this modeling.
So, what is this add command? This is a boolean command. So, whenever you are making a parametric modeling, you have to do the boolean operation only. What are the boolean operations? In the boolean operations, you can find assemble, remove, union trim. We will use these all commands one by one. But, for now, add command will be used. Now, again go to the body. Again go to the sketch. Click on the access system. Choose the point. Hit OK. Hit OK. Now, the inside diameter you have to define. Because, we have chosen the 2D as a 3. So, the D will be 1.5.
It is radius. So, I will make it diameter. Now, we will check exit from the sketch. I will again make a pad. And, increase this limit 1. And, minimize this limit 2. How much? Minus 2. Minus 2. Minus 2. This will give me a 4 mm gap. I am defining body 2. Right clicking on body 4. Going to the object. Choosing the boolean operation. That is, remove. I am just clicking OK. It is getting removed. Why I have not chosen the pocket. That I will tell you later on. During the big projects. So, you will get more clarity.
Compared to this big surface. My boss is looking very small. So, I am just gonna reduce the size to the. Now, my radius are there. And, drafts are there. So, I will define this body again. Go to the draft. Select the surface. Select the natural surface. And, draft has to give 0.25. Into T. So, this is my draft 1. This is 0.5. At the inside, I have to give 0.25 draft. Now, you can see. Now, you can see. You can see the shadow. So this can come out from the tool. There is not at all any issue.
After giving the draft, we will add some fillets. For the fillets, this will be my 0.5. So it's 0.25 into base thickness. That is again 0.5 and the inside will be 0.25. All right guys, all the dimension has been covered. It was not shown in the picture, but every time whenever you are making a boss, at least 0.5 chamfer has to provide it because we have made very small. So we can give 0.25 chamfer. This all are add-on features. So make sure after Boolean operation only, you will give this address of features. Okay. Now my boss is ready. I just rename this property from body2 to boss.
For good looking, I can give the radiuses here as well. But there is a thing which we should remember. If you are tooling guy or if you know the plastic industries, then you might understand, then there could be a sink mark issue because this having a more thickness here. So what we do generally here, just go into the pad command and increase this. Now you can see there will be no thickness or sink mark issue. In the next session, the same model, we're going to learn how to make it more parametric with the formulas. If you know the formulas, then it is good. If you don't know, just follow the next session.
So if you link with the formulas, then you don't have to go here. You just have to make the changes and the model will get updated automatically. So that I'm going to teach you in the next session. Thank you.
Part 3
Hi guys. In this session, we gonna learn about the parameters and the formulas. So in the settings sessions, I have shown you couple of settings which you have to done before using the CATIA. I will show you again here, go to the option, go to the infrastructure, part, display, and make sure these two points checked in. If you not have done during that session, just make sure, because in this session, if it is unchecked, you will not able to see these parameters in this tree. So make sure you have checked that button.
Now going to the next, as I shown you on the given picture of this model, they have given the values this as a T. They have not defined the value. So we have taken or we have chosen 2 mm for creating the model. What if they wanted to change this value? Okay. So if they ask me to change to 5, now what happens? My, this model is getting updated, but this length is not getting updated. Why? Because we have not created any link with this dimension.
So in this session, we gonna learn how to create such dimension or dependent dimension by which if I choose or if I change this value, the entire model will get updated automatically. So I just undo it for now. Control Z is the shortcut key for the undo. Now first we will define our T value. So click on the formula button. Here you just choose the length. By default it will become real. You have to change it to the length. Click on new parameter type. I will gonna change this name to T. This is my T.
For now, I am defining this value as a 2. Click apply. Hit ok. Here you can see a parameter menu appeared. This was not available previously. Now it is available. And here you can see the T. So you guys, one more thing I would like to add here. If this is T, you are simply looking at the T, there is no value you can able to see. I mean, if I wanted to check what value has been defined for the T, I have to just double click on it and then you can able to see the value.
To avoid this, just go to the option, tools option and general settings, parameters and measurement. Go here at the knowledge tab. Just click this two buttons. With value, with formula. Hit ok. And you are able to see the value now. You don't have to double click on it. This will help you to fasten your modeling. This is kind of shortcut here. Now I know this dimension is three times to the T. So what I am gonna do here is, let's just link the values now. I know the pad value is defined as a T.
I am not going to change anything in the sketch because this dimension is not given by any of the drawing. So this is my own dimension. If you are finding this value also given by someone or the industry or in your cat test, you can define this value in the parameter also. I will show you how you can create that link. But first, let's focus on the values which we have given by the drawing. In the pad, just double click on the pad and you can see there is a length. We have given 2mm.
How we can link this T to this T. Because this values are same. So, I will gonna right click on this. Make sure you are going to hit right click here. Go to the edit formula. And choose this T. Now you can see there is an icon. Now you can see there is an icon cam. That is a formula icon. And the value you cannot able to edit the value now. Hit ok. I will repeat this again for you. So you will be very clear. Double click on the pad command. Right click on this. Go to edit formula. And just choose this T. Don't do anything. Hit ok. And it's done. Click ok. Now you can see the entire model get red. That means it's been in update now. If I click on update, it will get updated.
Now I don't have to double click on here and change these values. I simply double click on this and change to 5. And control U is the shortcut for update. So I am gonna hit control U. So you can see the model get updated. Now again the issue is same. This is not getting updated. How we can change this one. So let's find out on dependency. This is pad 2. This is pad 2. Alright. So I am gonna click on pad 2. Right click here. There are two values. So I am just gonna right click here. Second limit we don't need.
So first limit. So first limit. Just gonna right click on the added formula. Again gonna click on this value. Multiply. Multiply. Multiply symbol from the num keyboard. You can put multiply. And just add 3. Click ok. And you can see formula icon has appeared here. And I can't change these values. Click ok. Update. So you can see your model is getting updated now. And it is linked with a single parameter. If I change this to 10. Control U. And you will get updated. You can see if I am changing this value. This parameters are getting fade. Why? I will talk about this on.
But first we will add some more formulas here. To maintain the relations. Just find out what common areas are there. For an example this radius is. Radius is 0.5. This radius is 0.5. So go to the formula. Again a new parameter type. Again a new parameter type length. With single value. Click on new parameter. And give a name. Radius. Ok. Now this radius. Just give it 0.5. Same thing you have to do here. Double click on this. Right click on this. Edit formula. Choose this radius. Hit ok. Ok. Before update. We will do the same. Here.
What you can do. Edit formula. Choose this one. Divide by 2. Hit ok. Ok. This one we have 2 mm. So we will left this as it is. And here we will add it again. Ok. Now all things has been done. With just 2 formulas. We can change the parameters. Or we can change the entire model. And it's very easy now. To get updated. Now. There was a difficulty. In this 10 mm. Let's just find out why it is happening. So you can see. So you can see. A champer command is getting failed. Because it is not able to find the edge. You can click here.
They are giving a remark. Edge not found. What does it mean? The catia is unable to find the edge. Let's see why it is. Because you can see. There is no pocket. Let's just make it again. As 3. Click update. And you can see there is a pocket. But. At 10 mm. It is. There is no pocket. Why it is happening. Because. In the remove command. We have not changed the value of this pad. So what I am going to do here is. So I am going to right click on this. Go to the added formula.
Go to the added formula. For it. Next funnel. Go to the added formula. Go to the added formula. Go to the added formula. Choose this T, multiply by 5, click OK and you can see 50 mm has been appeared with the formula. I am not going to change this one because this would be my minus one only because this is related to the thickness. So I am clicking OK, giving an update and you can see there is no syntax or something error is coming. All the things has been completed. It's all linked with this, just two parameters. You can change entire model with this two parameters.
So if it is 2, it will get updated. If it is 10, it will also get updated automatically. All right, guys. So and you can see the relations are came here. OK, so you can find out this relation what it is talking about. You have given fillet 1, fillet 2, fillet 3, paired, paired 1, 2 and 3. So it is talking about the relation what you have defined into this parameter. So this is all about making an parametric model. Now there is one more thing you can do at design table. How that is going to work. Next we will going to talk about that only and it will help you to create an Excel sheet linked with this model.
So you don't have to come in catia itself. So you don't have to come in catia itself. You just have to change the values of the T or radius into the Excel and this model will get updated automatically. So next we're going to talk about that one. Now let's see how we can create the design table. After creating the parameter and relations, it is very easy to create the design table. There is option of design table. Just click here. You can choose first create a design table with current parameters value. If you already have the design table with yourself, then you have to choose this one.
Because this is the first time we are going to create, I'm going to choose create a design table. I'm going to name it boss. Click OK. And it will ask you some parameter to get inserted. Which type of parameter you wanted to insert. So I am going to choose these two values because this is the only values on which I have linked my entire model because this is a small model. So I am going to choose only these two values. If you have multiple parameters, you have to choose those parameters as well. How you can choose it? Just click this arrow button. If you wanted to remove something, just click this back button.
Again, I'm adding the radius. Click OK. And it will ask you a path where you wanted to save your Excel sheet. So I am choosing desktop as of now. The name I have given already. Click on save. It will take some time. And you can see a configuration window has appeared. And you can see the two parameters is defining here. So if you wanted to change, just click on edit table. And that Excel sheet will be open. And they have defined what type of units you have and what type of parameter you have.
This parameters we have chosen and units we have already defined in MM. I am going to change it to three. And this I am keeping as it is. Before closing, just make sure you click on save button. Once it is saved. Close it. And Katiya will automatically take that synchronization. And this is the report. And it is showing that pause has been modified. Click close. Apply. OK. And model will be read because we have chosen the menu update. Click on update. And you can see the model has been updated automatically with the design table.
You can see the design table. You can see the design table at this portion. In the relation tab. If you want to change it again, just double click on this. It will open a configuration window again. Click on edit table. Change the value to the file. Change the value to the file. Click on save button. Close it. And wait for synchronization. Click apply. OK. And hit update. You can see it is getting updated very easily. So this is how you can create the parameters and relation.
And the design table also we have learned. So this is all for this session. I have given one challenge for this. You have to create the parameters and relation. So make sure you will complete that challenge. That will help you to create the parameters and relations. And it will be very easy for you once you are aware with this parameters and relation. You can create model very fast. And with a single click you will able to update the model. Thank you guys. We will see you in the next session.
Thank you.
Part 4
Hello friends, in the last session, we learned about creating a parametric model. So in today's session, we are again going to create two models, which will help you to create a lighting model. So we are heading over to the main depth modeling. However, this will help you to enhance your skill in the CATIA and you will be more aware about using of this CATIA. So we are going to use all those parameter design table to create these models. One is two-way locator and one is four-way locator. We also gonna talk about what is the use of two-way locator and what is the use of four-way locator, how we can use this in lighting and how we can create such locators in the 3D modeling.
So let's move to the CATIA. I have one surface here and you can see this surface has been made by me only for just your understanding. This is a circle and this is a hole. Okay. So first we gonna make two-way locator and then we gonna make four-way locator. What the two-way and four-way locator is? First we will try to understand that thing. Suppose you have the lamp and you want it to fit on the vehicle. So your position of mounting is not defined yet. If you are assembling the from the front side, so operator will not able to see which hole it is going or there is no connection.
Like if you have a pen with you and you have the cap of it, so you know you have to put the cap on the pen. But if you don't know where is the hole and where is the pin, you cannot able to insert that thing. Same thing happens on the lamp side, but it is having a blind hole. So for that we give the locators. Locator means to locate. I will create a model then you will understand more betterly what is happening. What I am talking about. So let's jump into the modeling itself. So first thing first, I am gonna make one point. Always create a point first. In any modeling, create a point.
In two-way locator, we gonna locate our lamp in two direction. In four-way locator, we gonna locate in all direction. So that's why it is called four-way locator. So in the oblong, you can see the x direction is free. Okay, we gonna just hold the z direction and the resting direction. That is the x. So first we create the point. To create a point, there are multiple ways to create the point. But we wanted to make our locator at this, the center of this oblong. So how we can create? Because finding a center of the circle, it is very easy. But here if I am clicking on this and choosing the circle sphere, then it will create a point here.
If I am selecting this as this, it will create a point here. And if I go to the here, it will not select any circle. So what is the best way? So best way is, just click on the point, drop down menu, click on curve. Choose this curve first and click on middle point. It will create the point middle of this line. Click OK. Same thing again at this portion. Click middle point, hit OK. Create a line between two points. You can see line type will be point to point. Click OK. Choose a point again on the curve. Choose this line this time and click on middle point.
Now you are able to, I just hide this point. Now you are able to create the locator on this position. So once I get my point, I will put my axis system on it to create the sketch. Click OK. So this all we have done in geometrical set as input surface. But if you are gonna do perfect modeling, then just make sure input surface should not be test by you. So what you can create is you can go to the insert, create a geometrical set and click OK.
You will get a new geometrical set. So now we wanted to shift this entire points into the geometrical shape too. What I will do, I just click on point 2, hold the shift and click the point 4. Right click on it, select object, change geometrical set, click OK and it will ask me for destination. So I am gonna click on this and click OK. You can see my points had been shifted to the geometrical shape. Now we can start our modeling. So first thing first, I will gonna insert one body because as I told in the last session also, part body will not be touched by you.
Because if the reason of not touching it, you cannot avoid to delete this body or you cannot avoid to change this body or you can't do anything with this body. So that's why we not choose this part body for creating any modeling. Just make sure whenever you are choosing the body, right click on it, define in work object. Choose the position sketch, choose the yz plane, origin type projected plane, we have already having. Now we will create a circle. So you can see the circle is going out of this boundary. So that means my radius is 10.
So we have created our circle. Now for the locator, the locator will look like a plus sign always. So the circle we have made to get our boundaries. We will create a line into it. So I will choose the best, the maximum condition and this maximum condition. Click OK. I will choose this again at a maximum condition and this maximum condition. Now what happens is if you go out, you can see the sketch is there and shift to the modeling, part modeling. Choose the paired command. Click OK. You will find an error. Why?
Because KTR will not understand the open boundaries. This is the open boundary for him. It will not getting understanding that you wanted to pair a circle or you wanted to pair this lines. Because this all are joined. So what is the solution for it? Just double click on it. Choose the circle and make it construction. By this way you have your circle, but if you exit from the sketch, it will be disappeared. Why? Because it is just for the construction purpose. So KTR will understand that you have created the circle just for your other geometry construction.
It is not related with the geometry. Now, again if I click on the pad, it will again show me an error. Why? Because in the paired command, it will only pair a closed boundary. But now we don't have the closed boundary. So solution for this is click on yes. Click on this thickness command. Now normally this thickness will be 40% of the base thickness. Base thickness is nothing as we learned in the last session. For the boss, we have defined the T value. So T is thickness. So 40% of the thickness.
If I have 2 mm as a base thickness, then 0.8 will be the thickness of this locator. So for now, I am going to choose 0.5 and 0.5. Why I have chosen thickness 1 and thickness 2? Let me show you what happens. If I choose the 1 mm here, you can see my point is here, but my entire model has shifted towards this direction. If I give the 1 mm here, and 0 here, then entire model will be shifted left to the point. So that's why 0.5 and 0.5.
Click okay. You can see the entire model has come middle of the point. That's what we wanted. Now we need to define the length. So length, as of now, we don't have any base here. So we can define the unlimited length. But at the top side, we have to make it defined, because you cannot create a big length here, because it might be possible that some part will come here, and it will be a crash condition. So we have to define the length of this at the top side.
At the bottom side, Bottom side, it will get merged. Let me create a dummy body for you for a better understanding. So I'm just going to click a body. Making a sketch. So this is my best boundary. I will rename it. Go to the properties and best body. So I have the best body. Now I have to define the height also. So what I will do here is I will go to the surfacing and this I am using the surface. surfacing because it will help me to create a parametric model in a best way. I am not using the same surface. I am creating a new extracted surface on it. And then I will choose the interim command. And I will select that extract. It will give me a warning. Click OK. Hit OK. Now you can hide your input surface. And you can hide the extracted.
How I am hiding it. How I am hiding it. I have defined in the session one that settings. So either you can choose that control one. Or whatever you have defined for the shortcuts. Or else you can just right click on this. And click on add button. Let me show you the best way. Let me show you the best way how you can find the shortcuts. By default shortcuts of Ketya. If you click on anything. Right click on anything. Or you can see there is a line shown on every font. I mean every alphabet. OK. What does it mean? It is a shortcut of that particular command. For an example. If I am right click here.
I will click R. That is this one. So it will reframe for me. I will click right click on this. And click O. It will open the property for me. If I right click on this. And click on D. It will ask me a delete command. So this one. So this is how you can find anything. Or if you wanted to find out the shortcuts for this. You have to click Alt. And then select the highlighted alphabet. For an example. If I am clicking Alt F. It will open me a file command. If I click on Alt E. It will open the edit command.
Again in the file. Again in the file. There are some commands available. If I click Alt F. And then S. It is going to save this. File for me. So I am going to save it now. To be located. Now I have this untrimmed surfaces. Why I have untrimmed it. I will show you. In few minutes. Now let me. Choose the offset. In the offset I am going to choose. The untrimmed surface. Let me choose first. The extracted surface. Which I have previously. I just hide this one. And I will define the length of this.
Boss. Or locator. At 5mm. This is my opposite surface. With the extractor one. For an example. I will show you again. I just. Give another color to it. Okay. This is my. Extracted surface. Or input surface. Which I had. I made. I made the offset of this surface. This is my. Offseted surface. With the 5mm. Length. Now let me. Try to cut. This body. With this. Obsetted surface. I will go to the solid body. Select the. Split command. And. Choose this surface. And. Which direction. I have to cut this body.
I have to. Keep. The downward. Body. For me. So I click. Okay. Now. Nothing happened. Because. There is. No. Cutting edge. Available. It is just. Pocket. Nothing is there. To cut down. Or there is no. Line available. To cut down. This body. Now let me. Show you again. If I choose. The. Antem surface. Click. Okay. And. Update this. Split. It will split for me. Because it is. Finding up. Surface. Body. On which. He has to cut down. The. This body too. So I just hide this.
Opposite it. Now. I will just open the. And hide the input service. So you can see. I have defined the. Height of this. Two way locator. At the bottom. We have the base. So in the base body. I will merge it down. I am going to choose. Boolean operation. I have already shown. The boolean operations. Add remove. In the last session. But in this session. We are going to learn about. The union trim. What union trim. Do for you. You can see. You have a body.
More than this boundary. But you wanted to keep. Only upper side body. And you wanted to remove. The bottom side boundary. What you can do. If you choose. Add command here. What will happen. Let me show you that one first. It is not going to delete. Any body for you. It will just going to add. As it is body. With the other body. If I choose the remove. Or assemble. Sorry. If I choose the assemble. It is also not going to do anything for me. If I choose remove.
What will happen. The cross. That body will remove. From the base body. Now let me show you. The union trim. I will delete this one. Define the base body. Just make sure. Whenever you are. Performing any boolean operation. You have to define the body. Right click on this. Union trim. Choose a face. To remove. It is asking. Which face you want it to remove. Suppose. I wanted to remove this face. I will choose this one. Click on the preview. It is showing that this face has been removed.
Rest of the things not been removed. And click OK. So this is how it works. Now. Is this model just completed? No. Because. You can see. There is a touching condition. In the blasting industries. There is no way to make. Such accurate part. In which they can maintain. This much accuracy. There are some tolerances. So for the locator. They consider 0.1 tolerance. And this part will also having some tolerance. 0.1 for this sheet metal. So we have to make sure. That at least 0.5 gap. Should be maintained.
So for that. What we can do here is. We because we have the parametric modeling. We just go here. And reduce to 9.5. Click on update. It will get updated. Now. Why this having a two-way locator. It is restricting. My. Z direction. By this way. And. It is free. In this wire direction. There is a space. To move this part. So. We have the movement. In the wire direction. And we don't have the movement. Into the Z direction. So that's why. We call it. Two-way locator.
Now. But only one thing. Is remaining here. We have to rest. This entire boss. Or entire locator. On this surface. Because. Suppose. There is no. Locking at this area. Then it. May be possible. That it will. Go more than this. Length. How you can. Make sure. That the part will not go. More than this. So for that. What we can do here is. We can add one more. Surface here. At this portion. To do it. I am gonna. Insert a new boundary. Choose my. X red plane.
Projected plane. Click ok. To make sure. That this boundary. Will be used. I will choose the. Element extracted command. And I will select the. Input surface. Click ok. It will give me the. Boundary of that surface. I am gonna. Isolate this one. Why because. First. We wanted to make. Entire surface. And for the safety. Purpose. We gonna split it down. So I am not gonna. Use this one. I just create. One new. I will pay it because we know we have 1 AM length and the limit 1 and limit 2 will be defined as a 0.5. Now we have our landing surface. To make sure that it having a limit till this end, what we gonna do is we gonna use the extract also untrimmed surface and right click on this, go to the split command.
Select the surface, select the direction, hit OK. You can see the surface has been shifted down. Now I will add this body. I will add. Or because this boundary is not more than this boundary. If it is more than this boundary, then we can choose the uniting command also. So now you can see there is a resting body also. So now we have a restricted surface in these X direction and we have restricted surface in Z direction. Y is free. So we can move our body in Y direction in this way. So this is called to be located.
Now one more thing. Every plastic body will have a radius and the chamfer because this gonna insert here. So to making that insert very easy, we will add some chamfers here for that. Like this we have added. Like this we have added at least 3 mm because we have the length of 5 mm. So we have added 3 mm into 45 chamfer. I will add few radiuses. To make sure it will add to someone. If it is sharp then the operator will get hurted. So to making it sure I need to add some fillets.
5 mm it is not taking. So we can try to reduce it down. As I said no sharp edges. So this is also a sharp edge. 0.5 is sufficient. And then we can define this radius also. Before that this radius also has to give a 0.5 is sufficient. And now my two way locator is ready. It is done now guys. So this way you can create the two way locator. Just save the file. Make sure whenever you are working. Keep it saving because we have turn off automatic saving.
So make sure you will save it manually. So this is how the two way locator works. So as I said this will restrict my z direction, x direction and it is free in the y direction. Now you can think out what will be four way locator will do. So for that I am just gonna save, make a save thing here. And rename it to the four way locator. This also I am gonna change. So let's move to the four way locator now. I hope this two way locator you understand. So four way locator making it very easy task for you now.
So first thing first, I am just gonna hide this body. Insert a new body. I need to create a point here. So because it is circle, it is very easy for me to create a circle. I am just choose the circle and click OK. Insert a sketch. Click OK. Create a body. Already I have. Sorry. Choose a position sketch. Top view. Go to the projection point. Click OK. Now I will create a circle first. This is also 10. And then I will choose this lens. Make it constructive. Go out. Make a pad. Yes. The thickness 0.5.5. It's good. And length. And we have the surface already with us here.
So first, we gonna make a split. What I am doing here is, I am adding this another body. So it will be, I can use the same body again. So I just copy and paste it at the bottom. If you are not understanding what happened here, you can rewind and see again. Or else, I will show you again here. What I does it, I inserted a new. Okay, let me undo it. And then again I will show you. This is my pad too, which is having a base body. So this is, it not having any, a boolean operation.
Because I have created the pad into the base body. To make a union trim, I right click on this. Go to the object and insert a new. What it will does for me, it will create the pad into a new body. And add a boolean operation. But this assemble, I am not want this assemble command. I just want to add. So I just go to the object and change it to add command. Because I have added a boolean operation, so our entire model will go into the update mode. And we click on the update.
Now I can choose this body as a separate for anything. I can do a boolean operation with this separate body. I can delete, I can make copies of this. So my current task is to make a copy. I defined, copied, go to the top of the tree and paste it here. So the same thing happened here. Now this body is separate. There is no link with this body. You can see there is no link. And this having a link with this sketch. So this sketch is separate.
Now, we have this body. I am going to rename this body first. Base4 locator. I am going to define this one first. Right click on the body 5. Choose the union trim. And remove. Click OK. You can choose any face for the removal. And there is no defined way. Now we have height. We have base. Next thing you know what you have to do. You have to make some chambers. You have to make another body for the resting. So I will create a body for the resting first. Pad it. 0.5. Limit to 0.5. And add into the body number 5.
Update it. I have added body number 5. I should add into the body number for the locator body. I have added here. Before adding. I need to make a split. So I have the untim surface. I just choose the split command and make a split. Click on update. This is all very basic guys. So you might be aware of this. If you don't know, then you can just open the video again and see it. How we are doing it. Here already I have shown for the 2B locator in very simple manner. So if you got stuck with this 4B locator, you should watch this one.
And here it is stretching conditions. So as I said, at least 0.5 should be maintained. So I am going to choose it 9.5. Click on update. It is getting updated automatically. And now we just have to add some jumpers. Alright, so now one thing. This body, the resting body I have added here. And that I have added here. Okay. There is no such requirement like this. It is just for the resting purpose. So you can add on this face also. There is no such requirement that you have to add in this direction only. But here what happens is if it is this gap is small, then if you add this body, it will eat more plastic material.
So to avoid that, you can just have the resting surface on this wall. Here there is no such requirement because all around it is same. So now we have the chamfer and we will add some fillets. In the plastic, make sure every sharp corner will have at least 0.5 fillets. 0.5 is the minimum requirement. And the more you can give, it is more easy for the tool maker. Always remember that after boolean operation only, you have to give this dress up commands. 0.25. Now it is okay.
So now you can't move this boss in this direction. I mean in the Y direction. And you can't move into the Z direction. And you can't even move to the X direction. By this only, you can say this is a 4-way locator. So if you are seeing that you are not able to move that locator or that path in any particular direction, then it is a 4-way locator. Or if you are finding a part can move in one direction, but it is not able to move in two directions, then it is a 2-way locator. So this is how concept works.
Hope this is very well understood by you and you are able to create the models now. So now next task is you to create a relationship between this and which whatever we have learned in the last session to create the relationship and the parameter design table, you can create same for this also. I'll just rename this one. So in your challenge, this is going to be your challenge that you have to create a relation and parameters and design table for this 2-way and 4-way locator. Hope this is very easy for you. Thank you.