Phil's ZW3D Corner
Awhile ago I got a ZW3D software request from Phil. He was interested in the purchase options. He downloaded ZW3D and within a month he was ready to purchase ZW3D Standard. He was highly interested in the surfacing capabilities of ZW3D. This was the beginning of a new adventure in 3D CAD.
I quickly realized Phil was not just some CAD
jockey he is also a professional Tool & Die Maker, Designer and Engineer.
Being a draftsman, Phil and I have quite a bit in common about standard
documentation and manufacturing. So not only will Phil offer tips on
modeling but in sharing his deep 3D knowledge as it pertains to engineering
3D CAD - Designing with Shapes!
Let’s do a project to show that you don’t need to use sketches to make a model in ZW3D. Often times I see many CAD users going straight to a sketch and I am baffled as to why. Sketching definitely has its place, but not for everything. I hope to show with this small project that you actually have other options. In this first example we are just going to focus on making a part, later I will show how we can make this part parametric without using sketches. One of the biggest problems with sketch based modeling is all the linked dependencies that are created with sketches. Why add extra dependencies if they are not needed. Another reason I avoid sketches is because sketches are very easy to break and if you don’t set them up properly based on design intent this problem is even worse. First let me show you a video of what we are going to do then I will walk you through it one step at a time.
We are going to use inches for this project. Let’s start with a block, under the Shape Tab select the Block Tool.
The block options dialog opens up and we see this:
As you can see we have a lot of ways we can control the block. A sketch only offers us a 2d shape which we then would still need to extrude into 3d space.
Select Center as the type then select the 1st Point and set to 0,0,0. Select Length and set to 3″, Width to 5″ and Height to 0.25″ as shown here and click the Green Check Mark to accept.
This simple shape only required one operation to create so it only leaves one Feature in the history tree. A sketch based approach would have left two Features in the tree, a Sketch and an Extrude. Some people would say ok what’s the big deal? Think of it this way, what if your part was made of 200 shapes and each one was made from a sketch…now we have 400 features in the History tree instead of 200. The time wasted over a large project adds up very fast. Not to mention the troubles you would run into if you edit a sketch early in the History Tree.
Ok, let’s move on.
Let’s select the Block Tool again and this time we are going to look at one way we can accurately place the block without a sketch.
You will notice in the screenshot that there is a drop down arrow next to the 1st Point Dialog Box. This is a drop down menu of Geometry Constraints we can use to control the placement of our Block. We are going to use the Along Constraint. What this does is allows us to select an edge and move the center point of our Block to a location along the edge by either a percent or an actual distance.
After selecting the Along Constraint set the dialog settings to match the screenshot and set the Percent to 35, then select your edge and click the green check mark like shown here.
Now we are ready to define the size of our Block. Set the Boolean to Remove and set the Length to 3.5″, Width to 1″ and Height to 1.5″ as shown and click the green check mark to accept.
Next we need to add a hole to our plate that is 1″ in from each edge of the top corner of our plate. To do this we are going to use our Cylinder tool using the Offset Constraint to locate the center. What the Offset Geometry Constraint does is offset X, Y and Z from a single reference point.
Next we want to select the Ref point we want to offset from and set X to 1″, Y to -1″ and Z to -0.25″ as shown then click the green check box to accept.
Now it is time to set the size of our hole and Boolean to Remove. Set the Radius to 0.375″ and the Length to 1″ as shown here and click the green check mark.
Let’s add our corner fillet to our plate. Select the edge shown and then select the Fillet Tool.
In the options dialog box that opens set the Radius R to 1″ and click the green check mark to accept.
Now we need to add the slot to the top of the plate, so we will create another Block and use the Offset Distance Constraint for the first point. What the Offset Distance Geometry Constraint does is offset a set distance from a reference point.
In the Offset Distance dialog select the Ref Point first, then set the Direction, and put 0.5″ for distance as shown here and click the green check mark to accept..
Now we need to set the size for the Block. Make sure Remove is set for the Boolean and then set the Length to 0.375″, Width to 5″ and Height to 0.375″ as shown and select the green check mark to accept.
Next we are going to look at the Points on Curve in the Wireframe Tab. This is a great tool for locating evenly spaced points along a curve or edge. In this case we are going to use it to locate two hole cutouts along the edge of our Plate. Click the Wireframe Tab and Click the Point drop down and select the Points on Curve Tool as shown in the screenshot.
Select the edge on the model and set the type to Create N Equally Spaced Points on Curve as the type and set the Number to 4 as shown and click the green check mark to accept.
Now that we have our center points that we can snap to let’s create our hole cutouts. Back on our Shape Tab select the Cylinder Tool and set the Center Point, Alignment Plane, Radius to 0.25″ and Length to -1″ as shown and click the green Check Mark to accept.
Repeat the steps from Step 7 for the other cutout and you should have something that looks like this.
Now we are going to add a chamfer to the edge of our Plate. We can select all tangent connected edges by holding down the Shift key on the keyboard and selecting one of the edges. After selecting the edge select the Chamfer Tool type to Chamfer and set the Setback S to 0.125″ in the option box as shown.
Now we are going to put a thru slot in the slot we created in step 5. To do this select the Block Tool and we are going to use the Middle Geometry Constraint to place the center of the Block. What the Middle Geometry Constraint does is locate the center of an edge.
Select the edge and in the Middle Constraint dialog box as shown and then click the green check mark to accept.
Next we need to set the Boolean to Remove then set the Length to 2″, Width to 0.5″ and Height to 0.125″ as shown and click the green check mark to accept.
Now let’s add the two fillets to finish off our slot. Hold the Ctrl key down on the keyboard to select the two edges show and then select the Fillet Tool and set the Radius R to 0.0625″ as shown and click the green check mark to accept.
Now let’s add the last Fillet to the slot. Hold the Ctrl key down on the keyboard and select the two edges shown and select the Fillet Tool and set the Radius R to 0.1875″ as shown and click the green check mark to accept. Now our slot is finished.
Now we are going to create the counter sink for our hole. Select the Cylinder from the Shape Tab and set the Center to the center of our previous hole and set the Radius to 0.5″ (Make Sure R is to the left of the green drop down arrow. This sets this value to a Radius and not a Diameter.) and Length to -0.125″ as shown and click the green check mark to accept.
We are going to create the pocket cut into the plate now using the Block Tool and the Along Geometry Constraint. Select the Block Tool and open the Along Constraint dialog box and select the edge and set it to Percent and set the Percent to 75 as shown here. You will notice I have been leaving some steps out and the reason for this is we are doing the same thing over and over, which you should know by now. If not refer to previous steps.
Now set the Block Length to 1″, Width to 0.25″ and Height to 0.5″ as shown and accept.
You might have noticed that the Width and Height are backwards in relation to our model orientation, this is because we didn’t set the Align Plane. We will talk more about that later when we set this model up for parametrics. I did this on purpose so I could show you what happens when you don’t set the plane alignment when using shapes to model. I would also like to point out that if you don’t set the plane alignment it will be easy to break your model with edits.
For now just know why it is this way and we will cover it better later.
Now we are going to add our peg to the plate using the Offset Geometry Constraint. Select the Cylinder Tool and select the Offset Geometry Constraint and set the X to -0.75″, Y to 1.25″ and Z to 0″ as shown here and accept.
Now in the Cylinder options Dialog set the Diameter to 0.5″ (Make Sure there is a Ø for Diameter and not Radius), Length to 1″, Boolean to Add and Align Plane to face shown here.
Add a fillet to the base of the peg that is 0.125″.
For our final step add a Chamfer that is 0.0625″ to the top of the peg and you should have a final model that looks like this.
In closing I hope this opens your eyes to the possibilities of modeling without always going to the sketch/constrain methodology. As I said before sketching has it’s uses just don’t abuse it just because that’s the way everyone else does it. In the next tutorial we will prep this model for parametrics and name things in the tree for easy editing later down the road. I hope you found this tutorial informative and useful.
Phil Procario Jr.
You can contact Phil directly at Phil@tecnetinc.com
Or contact TECH-NET at 206-842-0360 or email@example.com