Cam Catia v5 - Milling Tutorial 2018-2019 [PDF]

Zitiervorschau

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

CAM CATIA V5 Tutorial 1: Milling OBJECTIVES 1. To expose students with the CAM for CNC Milling Machine. 2. To teach student how to use CATIA software as a CAM for Milling Machine. 3. To teach student how to generate NC Code from CATIA for Milling Machine.

PROCEDURE STEP 1: MILLING PART PREPARATION

 TO CREATE MILLING PARTS 1. Once the Catia® is fully running, select Part Design under Mechanical Design menu. 2. By select X-Y Plane, sketch and modeling a milling part with dimension given as shown in figure below and rename the PartBody to Part.

CATIA® V5R21 Prepared by, Sanusi

Page 1 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

 TO CREATE STOCK PART 3. Insert new PartBody and rename it as Stock. 4. Select X-Y Plane or bottom surface of Part as reference to create stock part with dimension 100mm x 100 mm x 32 mm. 5. Select the Stock and change its properties by set the Transparency to 50 as shown below. Note: Stock is where your Raw material looks like Part is the shape that you want after machining process is completed.

Thickness of Stock is higher 2mm than Part

CATIA® V5R21 Prepared by, Sanusi

Page 2 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

STEP 2: POST – PROCESSING SETUP 1. Before you go further, you need to set the Post Processing for NC and its folder by going to the Option and select Machining.

2. Change the Post Processor and Controller Emulator Folder to IMS® 3. Create a new folder in My Document, and rename the folder as NC_Code. This is where the NC Code will be saved by Catia® 4. At NC Code: Select the folder that you just created. You should see the path below in the NC Code form. C:\Documents and Settings\Administrator\My Documents\NC_Code

CATIA® V5R21 Prepared by, Sanusi

Page 3 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

STEP 3: PART OPERATION SETUP 1. Change the workbench to the Prismatic Machining workbench by selecting pull down menu Start and then finding Prismatic Machining.

The prismatic Machining workbench will appear like figure shown below.

CATIA® V5R21 Prepared by, Sanusi

Page 4 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

 DEFINING THE PART OPERATION

2. Double select the Part Operation.1 branch in the PPR tree. This will display the Part Operation window. You noticed that there is no machine selected, no Axis setup and no part and stock selected yet.

3. Select the machine icon. Selecting this icon will display the Machine Editor window. Within this window you can define the machine that you will be working with for your part operation. 4. Click

the 3-axis Machine.1 machine.

CATIA® V5R21 Prepared by, Sanusi

Page 5 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

5. Click on the Numerical Control tab. Change the Post Processor to fanuc21i.lib. (This refer to our Milling Machine Controller). 6. Change the Post Processor words table to IMSPPCC_MILL.pptable (This refer to the coding style of the Controller) 7. Change the NC data type to ISO. (This refer to the NC format of the Controller) 8. Once everything is complete. Click OK button.

9. Next, select the reference machining axis system icon This will display the Machining Axis System window.

to set the Axis on the Stock.

There will be a red set of axes and planes in the center of the window. This axis system is how you define a new machining axis. By default, the machining axis appears at the central axis system for the assembly. Many times this will not be the right location. The axis will be moved to the back right corner of the table.

CATIA® V5R21 Prepared by, Sanusi

Page 6 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

10. Select the center point of the axis system. This will be the small red dot in the center of the axis as shown below.

The center red dot will allow you to move the entire axis system from one location to another. The Machining Axis System window will disappear and CATIA is waiting for you to select a corner vertex to be the new center of the axis system. 11. Select the top left corner of the table. This will define the new center of the axis. Select the corner shown below.

The Machining Axis System.1 axis will move to the corner. Notice the axis system turns green. This denotes that a new axis location has been defined. If the orientation of the axis is incorrect, you can select one of the axes and then an edge to define a new direction for the axis. 12. Make sure that the Z-axis is pointed to the TOP part CATIA® V5R21 Prepared by, Sanusi

Page 7 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

13. Select OK. This will define the new machining axis system. Next, the geometry will be defined. 14. Next, you need to select the Part and the Stock. 15. Select the design part for simulation icon. machining process.

This will define the final part of the

16. Select the Part in specification tree inside the ProductList and double click in workbench area.

17. Next, select the stock icon. machining from.

This will define the stock material that you will start

18. Select the Stock in specification tree inside the ProductList and double click in workbench area.

19. Select OK. This will define the Part Operation setup. CATIA® V5R21 Prepared by, Sanusi

Page 8 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

STEP 4: MACHINING PROCESS  FACING This will be the first section involving machining of a part. The order of the basic milling modes will be the order most commonly followed with any given part. First the part will be faced off or the excess material on the top will be removed.

1. Select the facing icon. The icon will highlight, but nothing will happen. This is because CATIA is waiting for the insertion point of the facing operation to be defined. 2. Select Manufacturing Program.1 from the specifications tree. This will insert the facing operation and tool change operation into the specification tree just after the manufacturing program.

Now the Facing window displays.

3. Next you will need to define some very important parameters. RED color meaning that the important parameter is blank or not correct. GREEN color meaning that the important parameter is set correctly.

CATIA® V5R21 Prepared by, Sanusi

Page 9 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

NOTE: Each tab also has a set of “lights” associated with them at the side of the icons. A RED light indicates that information needs to be entered. This denotes that CATIA does not have enough information to complete the tab. A YELLOW light indicates that the user has not defined any information but there is enough default information to complete the tab. You should always check these tabs to make sure everything is correct. A GREEN light indicates that all information is entered and is valid.



Geometry tab

4. Go back and take a closer look at the geometry tab for facing operations. 5. Select the top of the facing geometry. This will define the top surface of the design part that is to be created by the facing operation. The Facing window will disappear and allow for room to select the top of the design part.

CATIA® V5R21 Prepared by, Sanusi

Page 10 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

With the stock material shown, it will be difficult to select the top of the design part. 6. Zoom in and place the cursor over an area that you want to select for the top of the final design part. Below is shown a good area to concentrate on. 7. Press the up arrow on the keyboard. The peel selection will display. This is a utility that allows you to select faces, edges or bodies that are not on top.

8. Select the top of the final part face. That is, select the round dot in the center of the peel selection utility. The Facing window displays again, this time with the top and sides of the part turned green. By default, the boundaries of the top surface will be used as the boundaries of the facing operation. This is not the case since you have the stock material defined. 9. The other way is that you also can hide a Stock body directly in specification tree for more easy selection. 10. Select the plane in the contextual area. This plane allows you to define the top of the stock material.

CATIA® V5R21 Prepared by, Sanusi

Page 11 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

11. Select the top of the stock material. The plane will turn green when the Facing window shows again.

 Machining operation parameters tab 12. Select the machining operation parameters tab. This tab will be found for all machining modes. After setting the parameters for the first machining operation for a particular mode, the settings will remain persistent for the next similar machining operation. Even though the parameters will be the same, it is always a good idea to check them, watching for any new parameters or parameters needing to be changed. 13. Than select the Axial menu and change the Mode to Maximum depth of cut. This setting set the facing process to cut 0.5 mm per round.

CATIA® V5R21 Prepared by, Sanusi

Page 12 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

 Tool tab 14. Select the tool tab. If you remember, this tab allows you to define the tool that you want to use. Start by defining a facing cutter instead of an end mill. 15. Select the facing cutter icon. The image in the contact sensitive window will change to a facing cutter. If you are unsure of the parameters that you can define, refer to the introduction where all the facing cutter parameters are defined. 16. Double select on the Nominal Diameter (D) parameter and change it to 50 mm. This will make your face be 50 mm in diameter. 17. Double select on the Corner Radius (Rc) parameter and change it to 0 mm.

CATIA® V5R21 Prepared by, Sanusi

Page 13 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

 Macros tab 18. Select the macros tab. panel.

There are several parameters available in the macros

19. Turn on the Approach and Retract macros. This will tell CATIA that you are going to define both an approach and a retract macro in your machining operation.

20. Select the Approach and Retract Active and set the Mode Direct for both macro.

21. Click the Axial Icon

and change the Approach distance to 100mm.

22. Click the Axial Icon and change the Retract distance to 100mm. 23. Click Path Visualization Icon to simulate Tool Path. 24. Click the Simulation Icon and run the simulation.

CATIA® V5R21 Prepared by, Sanusi

Page 14 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

25. Select OK. This will take you back to the machining process.

CATIA® V5R21 Prepared by, Sanusi

Page 15 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

 POCKETING Pocketing cuts out the inside area of a part. Pocketing operations can also clear out an area, otherwise known as an open pocket but that will be investigated later. 1. Select the pocketing icon. operation.

As usual, CATIA needs a location for the machining

2. Select Tool Change.2 to insert the pocket operation after. The pocket operation will be inserted and then the Pocketing window will display. Make sure that the Pocketing Process is below the Facing Process. The sensitive area shown is similar to the ones you have seen before. There are some areas in red, like the bottom of the pocket and the boundary, and there are some areas that are a peach, or pink color. 

Geometry tab

3. Click on the Open Pocket to change it to Closed Pocket. 4. Click on the Top surface and select the Part Top surface. 5. Click on the bottom surface and select the bottom pocket at the Part.

CATIA® V5R21 Prepared by, Sanusi

Page 16 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

 Machining operation parameters tab 6. Go to the Axial menu and change the Mode to Maximum depth of cut and change the Maximum depth of cut to 1mm.

7. Go to the Radial menu and change the Percentage of tool diameter to 60%.

 Tool tab

8. Select the end mill cutter icon. The image in the contact sensitive window will change to an end mill cutter. 9. Double select on the Nominal Diameter (D) parameter and change it to 10 mm. This will make your end mill will be 50 mm in diameter. 10. Double select on the Corner Radius (Rc) parameter and change it to 0 mm. 11. The tool number is set as no 2 (T2 End Mill D 10).

CATIA® V5R21 Prepared by, Sanusi

Page 17 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

 Macros tab 12. Select the Approach and Retract Active and set the Mode Direct for both macro.

13. Click the Axial Icon

CATIA® V5R21 Prepared by, Sanusi

and change the Approach distance to 100mm.

Page 18 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

14. Click the Axial Icon

2018/2019

and change the Retract distance to 100mm.

15. Click Path Visualization Icon to simulate Tool Path. 16. Click the Simulation Icon and run the simulation.

CATIA® V5R21 Prepared by, Sanusi

Page 19 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

 AXIAL MACHINING

Axial machining involves all circular drilling type motions. The part just needs to be drilled, using several different drilling tools. The order in which holes are drilled is not as important as the order that a part gets machined. Usually drilling operations get performed last. 

SPOT DRILLING

1. Select the spot drill icon and then select Manufacturing Program.1. You have to select Manufacturing Program.1 before CATIA knows where to put the spot drilling motion. The Spot Drilling window will display. 2. Select the hole location sensitive area. This will allow you to define what holes are going to be spot drilled.

3. Select the four holes shown below. When selecting the holes you will not get a preselection showing you that you are going to be selecting the hole. You also do not want to try to select the edges of the holes, but instead, you want to select the inside faces of the holes. The order that you select the holes is irrelevant but will determine the order of the holes. 4. Double select in space. You have to double select on nothing to tell CATIA that you are done selecting points. 5. Change the depth of the hole to be 3.5mm. This can be accomplished by double selecting the value and then keying in 3.5. 6. There are still a few more pieces of information that you will want to add to the spot drill sensitive area. Next, you will want to define the top of the holes. 7. Select the top of the spot drill sensitive area. This will be the heavy pink line across the top. This will define the top of the holes. This is an optional selection because CATIA will assume that the top of the hole is the top of the material. Defining the top in this manner is especially important when the top of the hole is not the top of the material, as in the case where you are drilling holes before facing off a part.

CATIA® V5R21 Prepared by, Sanusi

Page 20 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

8. Select the top of the main body of the part. This will define the top of the holes. 9. Change the jump height to 10mm. This will make the tool jump 10 mm between each hole. Figure below shown a completed parameter selection setup.

10. Change to the tool tab and set the following parameters for a spot drill. This will make a small hole in each of the holes that you defined to spot drill.

11.Double select on the Nominal Diameter (D) parameter and change it to 5 mm. This will make your spot drill will be 5 mm in diameter. 12. Double select on the length spot drill (l) parameter and change it to 35 mm. 13. The tool number is set as no 3 (T3 Spot Drill D 5). CATIA® V5R21 Prepared by, Sanusi

Page 21 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

14. Change to the macros tab and add Approach and Retract macros that go to the safety plane. Remember, to do this, change to the tab, turn on the Approach and Retract check boxes and then select the add motion to a plane icon for both. 15. Select OK. This will finalize the spot drilling motion. Feel free to replay the operation if desired.

CATIA® V5R21 Prepared by, Sanusi

Page 22 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING



PPK Pembuatan 2018/2019

DRILLING

1. Select the drilling icon and then select the Spot Drilling.1 operation in the specifications tree. Drilling is your basic drill operation that will be used to drill the same holes that were spot drilled. The sensitive area for the drilling motion will look very similar to that for the spot drilling operation.

2. Select the four holes as same with spot drilling before. 3. Double select in space. You have to double select on nothing to tell CATIA that you are done selecting points. 4.Select the top of the spot drill sensitive area. 5.Select the top of the main body of the part. This will define the top of the holes. 6.Change the jump height to 10mm. This will make the tool jump 10 mm between each hole same as spot drilling. 7. Select the bottom of drilling hole to set a bottom of drill. Figure below shown a completed parameter selection setup.

CATIA® V5R21 Prepared by, Sanusi

Page 23 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

8. Change to the tool tab and set the following parameters for a drill. This will make a drill hole in each of the holes that you defined to drill.

9.Double select on the Nominal Diameter (D) parameter and change it to 8 mm. This will make your spot drill will be 8 mm in diameter. 10.The tool number is set as no 4 (T4 Drill D 8). 11.Change to the macros tab and add Approach and Retract macros that go to the safety plane. Remember, to do this, change to the tab, turn on the Approach and Retract check boxes and then select the add motion to a plane icon for both. 12. Select OK to finish the drilling operation. Again, do not forget to replay your operation to make sure it performed as you expected.

CATIA® V5R21 Prepared by, Sanusi

Page 24 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

STEP 5: GENERATING NUMERICAL CONTROL (NC) CODE 1. Once everything is completed, it is time to generate the NC code. Click on the Manufacturing Process.1 and select Generate NC Code Interactively.

2.A Generate NC Output Interactively windows will appear. 3. Select NC data type as NC Code and select as by program. 4. Choose directory file for Output File and CATProcess after NC data generation and then select Execute.

CATIA® V5R21 Prepared by, Sanusi

Page 25 of 28

EPT 181 CAD/CAM CAM TUTORIAL 1: MILLING

PPK Pembuatan 2018/2019

5.A IMSpost – Runtime Message windows will pop-up. 6. You will be required to enter the Program No. Enter any number that has four (4) digit (0001 ~ 9999). 7. You can change the Program Start and End command for the NC Code that suit the CNC Milling machine at the NC formatter.

CATIA® V5R21 Prepared by, Sanusi

Page 26 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

8.Finally, check your NC Code in the NC_Code folder that you created earlier in this laboratory exercise.

CATIA® V5R21 Prepared by, Sanusi

Page 27 of 28

EPT 181 CAD/CAM

PPK Pembuatan

CAM TUTORIAL 1: MILLING

2018/2019

QUIZ 1. Create and simulate the part below and save the NC Codes based on milling process that you select. 2. All dimensions are in mm.

-------------END-------------CATIA® V5R21 Prepared by, Sanusi

Page 28 of 28