Mechanical

Uploaded on

26 Dec 2022

Skill-Lync

This article will take you through a much simpler method to isolate sketches before projection in the Sketcher Workbench in CATIA. The conventional method is a time-consuming task, especially if we want to select multiple projected edges and then right-click to isolate them. Therefore, here’s a simpler method to isolate it using one button before projecting it.

Select the edge that we need to project and click on Create Datum first, and then click on Project 3D Element.

**After that, you need to constrain them properly and make the full sketch as per iso constraints.**

But this time when you constrain with the steps and methods we learned in constraining a rectangle, we came to know that it is still under constraints when we check the sketch-solving status bar. This is because, when we create a rectangle, some geometrical constraints like horizontal vertical, coincident, concentric etc, will happen automatically. But when we isolate and project a body, these properties won't exist, and you need to give geometrical constraints separately.

Finally, use the **Trim** option to join them together

Let’s see another example where we project the edge as a construction element. You may wonder whether the same procedures like ‘isolation and constraining’ are required for construction elements. The answer is YES! Always isolate the sketches, even if you are using them for construction and constrain them again.

Let's take the following situation. If I need to create a stiffener here, we would first need to create a line connecting both. To do so, we use the help of projected construction lines.

So we take the appropriate plane and project the element using the project 3d element tool.

Here we made the projected element as a construction element. For now, I am not isolating it. Now, let's create the stiffener.

Now, if I come across a condition in which my stiffener needs to be in its same position and dimension, but two side-wise supporting blocks should have equal length, let's see what will happen if I modify it.

So what happened here is that my stiffener also got modified when I modified the support blocks. This confirms that even if we use the projected elements as a construction, they will maintain the same relation properties. In the case of stiffeners, you can follow this method as we want them to be in relation to the body.

Let's get back to the original position.

If we go back to previous examples, we notice that the projected element is actually a part of the sketch. But here, we are only using it as a construction element for locating the line used for the stiffener. So here, we are not directly using the projected element for the stiffener command. But we need its help to locate the line's actual starting and ending point. So, indirectly it is a part of the sketch which brings a parent relation along with it.

Either we can go with our usual method to isolate it and constrain the construction element. But the question here is, is it necessary to do so? No.

However, what we can do is delete the construction element, as we know that by doing that, we are not disturbing the actual position of the line.

By doing this, we now see that the line is not constrained fully. Because it was previously constrained with the help of projected construction elements, and they are no longer there in the sketch.

So we need to constrain the line manually from horizontal and vertical without disturbing the line position.

Let's see another example where we use the projected element as a construction element.

We need to create a new circular sketch of dia, 20mm from the centre of the hole.

As a first step, we will project the inner circle using Project 3D Element and make it a construction element.

Then we will select the point option without clicking anywhere. Perform a right-click on the construction circle and select the concentric option.

Now we will have a centre point for creating our 20mm dia. circle.

Delete the projected construction element and constrain the point from the horizontal and vertical axis.

After that, make the standard point into a construction point**( Note:-If we do not make a point into construction, it won't allow the sketch to form a solid while doing a pad operation) **

Now we have a centre to draw the 20mm dia. circle. Not that, in the above two examples, breaking a relationship is not necessary. These are the situations where we needed them to have a relationship with the parent. Here is the possibility that we can also delete them if required.

**Error - Feature Involved In an Update Cycle, **the next example will indicate that we need to break the relation of the projected construction element to achieve the required result.

**Note:- This you need to be worried about only after learning Boolean.**

The required result and current progress of the situation we are dealing with is shown in the above images.

Now the only operation remaining is to pad two stands left and right of the main body.

For that, we will create two similar rectangular portions by referencing our main body. Here, we will first project the outer edge using a project 3d element and then make it into construction. Now with that reference, we will create two similar rectangles.

We are projecting it because we want the exact outer edge for drawing the two rectangular sketches.

Now, we will insert a new body and will pad it.

The actual problem arises when we try to use the boolean add to join the newly extracted pad with the main body.

After updating the new boolean operation, we will encounter a new error mentioning **‘Feature Involved In an Update Cycle’. **

This error can occur in some other situations too. But here, the reason for this error is due to the related issue that happened when we projected the edge from our previous body.

How can we rectify this error? Click on the edit option for the sketch that is showing an error. Here it is, sketch 3 having the issue.

Just select those 3 projected construction elements and delete them.

Now constrain them again properly without disturbing their actual position. Make them iso-constrained.

Now we need to go back and update the model for the final result with no error. What we did here is that we are removing some unwanted relations so that the update cycle can perform without any error.

Here, this example is not focusing on creating the entire sketch. We will focus on how to create those two fillets attached with circular and rectangular portions.

After completing the above sketch, we need to create a circle of R36 in a random space.

Next, make the two selected portions of the sketch below tangent to each other.

Now, drag and place the circle closer to the image shown below.

Now click on the circle of R36, click on the fillet R18 closer, and add the fillet of R5 between them.

Trim the extra portion on the circle.

Now make fillet R5 tangent with fillet R36. Now coincide the end point of fillet 36 with the R10 circle. Also, a fillet of R1 is given between the R55 and R10 circles previously. So, while coinciding, we are actually coinciding with the endpoint of the fillet R36 with fillet R1.

Also, note that the previous tangent condition we provided with R36 and big circle R55 is lost for some reason. We need to reroute the tangent condition again by selecting them and giving the tangent back.

Now just give a horizontal dimension between the midpoint of fillet R5 with the vertical axis. Now mirror this towards the other side and also do the necessary changes required like changing the sideline/edge of the rectangular portion to construction etc.

Author

Navin Baskar

Author

Skill-Lync

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