Datum Tutorial Part: Cutter

Transcription

1 Datum Tutorial Part: Cutter Objective: Learn to apply Datums in different ways Directions 1. Datum Axis Creation a. First we need to create a center axis for the cutter b. Model Tab > Datum > Select Axis Icon Axis Icon Datum Axis Pop-Up Menu: Shows Datums, Edges, or Surfaces the datum axis references. NOTE must have two references c. Select the Right Datum: This will show the datum axis on the screen along with two locator markers (Green Boxes). We will use an existing datum to reference off of. Reference Markers

2 d. Hold CTRL (Control) button > Select Top Datum > Click Ok Axis between the Right and Top Datum known as A_1 2. Creating an Angled Datum NOTE: must have at least two selections (In this case Axis and Datum) a. Model Tab > Plane Icon > Select the Axis A_1 b. Hold Control > Select Right Datum 1. Select Axis A_1 2. Hold Control Select Right Datum 3. Check the reference measurement is coming off of: Change Rotation to 60 from or Top or 30 From Right 3. Building the Base part of the cutter a. Model Tab > Extrude > Select Front Datum > Design the following sketch 1. Create a reference circle with dia. 8 > Change to Construction 2. Create the following 3 Circles of equal Dia Trim the interior intersection of the circles Optional ways to associate the selection: Through- Passes through selection Offset- Allows to change distance or angles based on selection Tangent- Make a datum tangent to a surface Normal- passing through or parallel to selection Parallel- Makes datum parallel to selection. Be sure to line up the center of these two circles Trimmed Interior

3 b. Green Check to accept the sketch > Extrude distance 2 c. Complete part d. Drill a simple hole in the center with a dia First Tool: Offset Datum The first tooth will be the one at the right (3 o'clock position). The design intent for this tooth is that the inner side of the tooth will be a specified distance away from the disk axis. We will create a datum plane at the desired distance that we can use as a sketching plane. The tooth will be extruded outward (for a fixed distance) to the outer edge of the disk. Then we will place a hole, also on the new datum plane, using the both sides option to go radially inward and outward. a. Model Tab > Plane Icon > Select Right Datum > Offset Value 8 > Click Ok b. Model Tab > Extrude Icon > Select Datum 2 c. Select the Vertical Sides of the Base as References > Sketch the Following Profile Top Datum/Axis A_

4 d. Select Green Check > Extrude Distance 2 > Select Green Check Datum 2 e. Creating a hole i. Model Tab > Hole Tool > Select Datum 2 > Drag the Green Locators to the Front and Top Datum > Set the offsets to the following 1. Front Datum Offset 1 2. Top Datum Offset 0 3. Hole Diameter = 1.00 (Same Diameter for all 3 Holes) 4. Change Extrude distance from Blind to Symmetrical About the Datum a. Drag the distance so the hole drills through outside of the base to the center hole of the base (Recommend to change view screen to wireframe or no hidden to get a better visual of where things are located)

5 5. Second Tool: Normal and Tangent Datum The second tooth is the one at the top left of the part. The intent demonstrated here is to have the planar outer surface of the tooth tangent to the arc of the disk and to extrude the tooth inwards towards the center of the disk. So, we will create a datum to give us a flat sketching surface at the outer edge and tangent to the disk. We can make use of our existing datum DTMI which passes through the center of the disk and the second arc. a. Model Tab > Plane Icon > Select the outside surface of the top left arc (Change datum option to Tangent) > Hold CTRL Key Select DTM 1 > Select Ok 1. Select highlighted surface 2. Change Datum Option from Through to Tangent 3. While Holding Control Select DTM 1 b. Model Tab > Extrude Tab > Select DTM 3 > Draw the following profile (Recommend to change view screen to wireframe or no hidden to get a better visual of where things are located) > Sketch the same size profile as Tool 1

6 c. Green Check > Change Extrude Distance to 2 > Make sure the extrusion goes towards the center of the Base d. Drill a hole similar to the hole located on the first tooth 6. Third Tooth- Making Datums on the Fly The model is getting pretty cluttered up with datum planes which is making it more difficult to pick things out on the screen. One way to deal with this, of course is to just turn off their display. This gets rid of them all, which cleans up the display but may make selecting them or difficult (you could always use search to find them or use the model tree). A more selective way to scrolling their display is to Hide them' Do that now with datum DTM1 - select the datum and then at the bottom of the RMB pop-up menu select hide. The datum disappears, but not its children! Do the same with DTM2 and DTM3 (use CTRL-click to select them both at the same time). The default datums should still be visible. Open the model tree and observe the gray box on the icons for these datums that indicates they are hidden. All the datums we have created up to now have taken their expected place on the model tree. If a datum is only going to be used once to create another feature, it seems wasteful to create one that will be a stand-alone permanent feature on the model tree. Furthermore, we would likely want to hide it to get it out of our way. The solution used by Creo for both these problems is a make datum. This is a datum that is created just when needed ("on-the-fly"), and then is automatically hidden when the feature using it is accepted. Make datums are sometimes called "datums-on-the-fly" for precisely this reason. The new terminology for make datums in the Creo release is "asynchronous datums", which is a bit of a mouthful. We will continue to use the old terminology. One other new facet of make datums is that they are listed on the model tree, but in a special way which we will soon discover. The rules and methods for constraining a make datum are the same as if it was a regular one. What determines whether a plane is considered a make datum is when it is made. All our previous datums were created before we launched the commands that used them as references. For example, for the first tooth we created DTM2 first, then picked Extrude, then identified DTM2 as the sketching plane. For a make datum, this sequence would be changed: pick the extrude command first, then when we are asked to identify a sketching or reference plane, make the datum" on-the-fly". This is sort of a 'Just-in-time" delivery notion.

7 We are going to do other things in a slightly different order for the third tooth, by creating the hole first. However, a hole requires a planar surface for its placement plane. We don't have such a plane at the desired angle. So, we will create the hole using a make datum to act as the placement plane. Proceed normally to start the hole creation - that is, select the Hole toolbar button. You are asked (see the message area) to select a placement plane - but there isn't one in a suitable orientation. Here is where we will make the datum on-the-fly. Select the Datum Plane button in the Model Tab. The hole dashboard is grayed out, and the Datum Plane dialog window appears. We need to specify the constraint references for the new datum. Select the reference A_1 of the cutter. This is entered in the Datum Plane window with the default constraint through (just what we want). Now CTRL-click on the TOP datum. It is added in the Datum Plane window with the Offset constraint with some rotation angle assumed. Change this angle to 30 degrees below the TOP datum, as shown (you may have to use a negative angle). When this feature is finished, select OK. NOTE DTM 1, 2, and 3 are greyed out because they have been hidden

8 We can continue on with our hole creation. Select the hole tab at the top of the dashboard (the only button active) to return to the hole creation. A previewed hole will appear on the new datum plane (which is called DTM4). Set the diameter to 1.0 and the Depth Blind to center. Now drag the linear reference drag handles to FRONT (you can drag to anywhere along the displayed edge) and Axis A_1. In the Placement slide-up Datum Planes and Sketcher Tools, change offset to Align for A-1 and Offset for Front. The hole preview is shown below. Set Front Reference Offset Value to 1.00 Change option Offset for A-1 to Align (Click on the word offset to give the option menu. This will make a zero offset Part with third hole Completed When the hole is accepted, there is no sign of the make datum we just created, although the hole does have an axis. Open the model tree. The other datums are all there (some are hidden), but the make datum DTM4 is not. However, the last feature on the model tree must be the hole we just created. This is shown as a group. Open the group by clicking on the "+" sign, and there is our hidden DTM4 along with the hole that used it. If you select it in the model tree, it highlights on the model. Right click on DTM4 in the model tree and select Edit. You will see the angled dimension associated with this make datum. Now create the last tooth. This will also be a sketched protrusion on a make datum that is perpendicular to the axis of the hole (that's why we made it first) and tangent to the cutter surface. Select Extrude > Placement Tab > Define 1. Placement Tab 2. Click Define

9 The Sketch window is waiting for us to specify the sketching plane. Move it (the Sketch window) out of the way and select the Model Tab > Datum Plane button. Select the axis of the hole we just made, and (using CTRL-click) the surface of the cutter where the hole comes out. In the Datum Plane dialog window, set the constraints or these references in the pull-down lists to Normal (for the axis) and Tangent (for the surface). The preview should show a datum plane at the correct location and orientation. See Figure 24. Accept this datum and return to the Sketch window. 1. Select Axis of Hole 2. Hold CTRL > Select curved surface 3. Change Constraint type a. Hole = Normal b. Surface = Tangent Set the view direction away from the center of the cutter using Flip. Use Front as the Left Orientation reference plane for the sketch. Now select Sketch. Once again, check your view orientation relative to the part. Pick the existing tooth edges as references, plus the front and back of the cutter body. Since these are all parallel, you are still only partially placed. For the final sketch reference pick Axis A_1. Sketch the tooth as shown below. Note that in order not to fill in half the hole through the tooth, we must sketch around the circumference of the hole. Use the Project button is handy for this. Select this command and pick the curved edges of the hole, lines will be drawn over these existing edges. You may have to pick edges on each side of the circle, and come back later and trim the edges away.

10 Project When sketch is complete, set the Blind depth to 2. We have now finished constructing the part, which should look as follows. NOTE all of the teeth are pointed in the same direction. Save and show Teacher completed part.

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