Presentation is loading. Please wait.

Presentation is loading. Please wait.

CNC machining for D&MT:

Similar presentations


Presentation on theme: "CNC machining for D&MT:"— Presentation transcript:

1 CNC machining for D&MT:
Week 4: HSMWorks 01 Philip Dixon, Technical Instructor

2 Aim of this session To provide an overview of the processes required to progress from a designed component to a CNC milling part program

3 Intended learning outcomes of this session
Knowledge and understanding: by the end of this session, you should be able to: Effectively manage your manufacturing files Assemble your component for part programming Begin programming Practical skills Assemble and program a component

4 Design timetable (CNC element only)
Week Wednesday/Thursday, Activity 1 (AE) Intro: Module overview Intro to CNC control in manufacture 2 (AE) Engineering drawing for DMT Drawing refresher ASM section views GA’s and BOM Applying tolerances Doc management and export to PDF 3 (AE) CAD for DMT Data management Assembly modelling Plastic Advisor 4 (PD) HSMWorks 01 Project setup and management Tooling Milling cycles: Face, Contour 5 (PD) HSMWorks 02 Pocketing, Rest milling, Drilling and engraving Post processing, Setup Sheet

5 Starting our part program
Copy “XYZ VMC560 Template” from TeachDoc-LDS>CNC Machining Templates>Solidworks There is a template for each CNC machine, we will use the template for the XYZ VMC 560 machines. Copy to Desktop Copy the top block part from DMT week 03 and drop into our newly copied folder. Note: this will create a copy, it will not update if changed!

6 Open this in Solidworks, this is our manufacturing file.
It is defined as the table on the XYZ VMC560, don’t worry that we will be proving this on the Denford first, we can use this for both, you don’t need to do it twice!

7 The material stock should be representative of the material you are starting with. Our sample part measures 150x100x25 when finished. We want all sides to be machined so our material is 153x100x25.4 (we have machined the 100 Dim) Open the material stock and change it to the size of your starting material. Make sure the NC_WP_ZERO is correct!.

8 Assembling your Component
Assembling your component is the same as adding a component to any assembly. Think about your design intent! Our part finishes at 25mm and our block is 25.4mm. it is tempting therefore to assemble our part 0.4mm below the top surface. This is not what we want to achieve though: Imagine that you go to the shop and they only have 30mm thick material. You change the material size in our assembly but our part is still 0.4mm below the top. We machine a part 29.6mm thick! This is NOT our intention. We should instead assemble the bottom face coincident to the bottom of the block, thus if we had thicker material it would still machine to the correct thickness. This is our design intent.

9 Assemble your part into the material stock
Assemble your part into the material stock. Allow material for machining on the ends by assembling with a distance of 1.5mm ( )/2 = 1.5mm to remove each end. Assemble the block coincident with the bottom of the stock. If you are machining an insert you may need to assemble with a distance from (or coincident to) the top especially if you are holding on excess material. Distance 1.5mm Coincident Coincident The part should be fully constrained before you proceed. You need to constrain the 6 limits of freedom : 3 Axial, 3 Rotational.

10 Setting up the part program
From the CAM tab, select Job. If the CAM tab is missing you may need to turn on MPF from the Tools>Add Ins menu. MPF by default attempts to create a stock box around the model, we already have stock modelled as a solid so select From Solid from the drop down box, then select our material stock model Select the model we wish to machine in the model box, ensure you select only the required model Select the zero point, by default you should be using the NC_WP_Zero

11 Our first machining step!
Machine the thickness by facing the stock to the top of the part. Select the Face cycle from the 2D milling drop down box on the command bar. Select the facing tool from the tool library The side bar contains all of the settings required to define the cycle, it is best if we just run through the tabs left to right. HSM will attempt to create a cycle regardless. If in doubt accept the defaults and change it later.

12 A quick word about tooling
At first it may seem to make sense to create our tools and number them in the order we are using them: T1: Ø80 Face Mill T2: Ø10 Slot Drill T3: Ø2.5 Slot Drill T4: Ø5.8 Drill T5: Ø6 Engraving T9: Ø80 Face Mill T1: Ø10 Slot Drill T6: Ø2.5 Slot Drill T3: Ø5.8 Drill T4: Ø6 Engraving Tool Carousel gives us this Our tools are held in a carousel and are already predefined. We save a lot of time if we use existing tooling where possible and their current locations. Each physical tool must have it’s own tool number. You may reuse tools any number of times and in any order, you don’t need to redefine or give a new tool number.

13 Tool selection Large areas should be machined with a large tool Remove smaller areas afterwards with the appropriate tool Maximum cutting depth is 1.5 x Ø Maximum cutting step is 2/3 flute length 2.5xØ SO: Ø2.5mm slot drill: Max depth 3.75mm, cutting step 3mm Ø10mm slot drill : Max depth 15mm, cutting step 10mm 1.5xØ

14 Clicking the Tool Library button opens a list of predefined tooling, we can add tools, edit, set default feeds and speeds and set the tool holder from here. Select tool #9 Ø80 Face Mill from the list of available tools. If we revisit this library it will show what tool is used for any defined cycle. As this is the first cycle we’re defining, the tools are blank in this regard.

15 Select the defaults for feed, speed & coolant
Select the defaults for feed, speed & coolant. HSM has correctly identified the outer boundary of the stock as the area to machine. Go to the passes tab and change the stepover to 60mm and extend the pass 25mm each end.

16 Checking our work It is best if we check our newly defined cycles as we go, to do this HSM will simulate the selected cycles. If you wish to simulate multiple cycles, select them too. You can also simulate the entire job by selecting the Job folder itself. Highlight Face1 and then select simulate. The radio buttons will run the simulation. You can change the speed with the slider bar (or even make it run backwards) To simulate the machining rather than just the path the tool takes, check the show stock box.

17 Machining the left side to size
Contour milling Machining the left side to size To machine the left side we will use contour milling. Select it from the drop down box just as we did with the face milling cycle, select the Ø10 slot drill from the tool library. Note: we can’t machine the right side as the cutter would hit the vice!

18 In the Geometry tab, select the edge to machine
In the Geometry tab, select the edge to machine. This should be the lowermost part of the model i.e. as deep as you want the cutter to go. Make sure you have Propgate along Z unchecked. Check the arrow is to the outside of the profile. If it isn’t use the reverse button to make it so.

19 If we leave the cycle as-is, the cutter will attempt to machine all of the contour depth in one pass. This is not possible. To change this we can define multiple passes to reach the depth. Add 5mm to the ends of the cut (as we did with facing to prevent the cutter starting on the exact end of the part. Under the Passes tab, check the multiple depths box, enter a value of 3mm in the roughing depth box. Ensure that Stock to Leave is unchecked.

20 Adaptive Clearing Roughing out the main cavity
Using our Ø10 slot again select the inner, lower contours of the cavity. Be sure to select all the islands. Failure to do so will result in them being machined away. Unlike the contouring cycle definition, keep propagate along Z checked to chain all of the profile. As always pick the lower contour.

21 As we are roughing out the cavity only, we leave material for finishing.
Under the Passes tab, make sure Stock To Leave is checked. Allow 0.5mm on the sides and 0mm on the depth for later finishing. It quickly becomes apparent that the tooling chosen will result in areas not machined. We will remove this material at a later stage. It is better to do this rather than just use a small tool to clear all the area.

22 Adaptive Clearing Roughing the open slot
In order to make sure the end of our slot is fully machined into the existing roughed cavity, we create a sketch on the lower surface to define the closed area of the cavity. Note the fully open end is left open. Using the same tooling and cycle as for the closed pocket, we can define the open slot by just selecting the 3 sides of our sketch. Make sure Propagate along Z is unchecked and that the arrows point inwards. As before we will leave 0.5mm side stock for later.

23 Defining New Tooling New tools can either be defined from the tool library button in a cycle or from the tool library button in the command bar. We are going to define a Ø3mm slot drill for use when removing the remaining material from the main cavity. From the dialog box, select New Mill Tool If you enter the default feeds & speed here. You can always alter this in the cycle definition. Enter the tool number. Remember 6,7,8 &12 are free. Add the cutter profile info. Most critical are the type and diameter. You can just accept the defaults for the rest.

24 Pocket Milling Finishing roughing the cavity by rest milling
Rest milling allows us to revisit a previous area and remove additional material where possible. Select the newly defined Ø3mm slot from the library. As in the adaptive clearing, select all of the features of the cavity. Check the rest milling option and tell the system what size tool was previously used to machine the cavity. In this case it was Ø10mm with a corner radius of 0.

25 As Usual HSM will attempt to machine the remaining material in one go
As Usual HSM will attempt to machine the remaining material in one go. This will break the tool. Go to the Passes tab and check Multiple depths, set this to 1mm passes. Also due to the narrow gap, we can’t leave finishing stock so uncheck the option. We could use a yet smaller cutter but ideally we want to use the largest possible. When we accept the definition the tool has only cut the area the previous tool didn’t. In other words, it’s machined the rest.

26 Finishing the Cavities
Profiling using 2D contour As we made sure to machine the cavities to depth, only the sides require finishing. To do this we’ll use the Ø3 slot drill. As before, select the contours to machine making sure the arrows are to the correct side of the line. Notice that in this definition there are multiple depths. Ideally we’d machine most of the sides with a larger cutter and only use the 3mm for the small island and surrounding area

27 Drilling The Holes Drilling using hole making cycles
All of the drilling cycles are in the drilling drop down on the command line. Select drilling. From the tool library, select the Ø5.8mm drill. Although the holes are Ø6mm in the model, HSM doesn’t really care what drill you define. Select the 2 holes in the geometry tab. As we are sat on parallels (or the vice base in the case of the Denford) only drill 10mm deep. From the Heights tab, alter the depth to be -10mm from the model top. Ensure Drill tip through bottom is unchecked otherwise it will add the point height to the total depth.

28 In the passes tab we can define the drilling cycle type
In the passes tab we can define the drilling cycle type. In reality we only need to consider 3 cycles: Drilling- rapid out Drills straight into the material, perfect for these holes. Chip breaking – partial retract Will drill to a depth and then retract slightly to break the swarf. Deep Drilling – full retract Use if you are drilling a small hole (say Ø4 or under).

29 Trace Milling Milling the Sprue
To mill the sprue, we’ll use a sketch to define the path. Define the missing tool #5 Ø3mm ball nose. Select the line as the path, the arrow should be pointing inwards, this is so we start outside the block and mill inwards.

30 Important! In the passes tab, make sure compensation direction is set to
Center. Failure to do so will cut the sprue in the wrong place! Our preview shows the cutter will successfully machine the slot. Note that the end point is the centreline of the cutter. the slot will therefore be 1.5mm longer than the line. As we are working from a 2D sketch, MPF cannot work out the depth of the slot. To define this we tell it to move the axis -1.5mm (the depth of the slot)

31 Engraving The Text Trace Milling
As we saw previously, we don’t even need CAD geometry to be able to create a cutter path. Let’s engrave the missing lettering by defining a sketch and setting up the trace as previous. We’ll use tool #4 for this and set a depth of -0.25mm using the axial offset as before. Note that HSM correctly differentiates between construction lines and solid lines thus picking the sketch will select the correct path. As before make sure the compensation is set to center.

32 Stock Simulation Checking our work so far
So far we’ve been using simulate to check our work, now we’re going to check our cutter paths and also verify against our model to ensure that all is correct. Highlight the job (or select all the cycles) and select Stock Simulation from the command bar. All of the play buttons should be familiar. It is also telling us the total machining time is 10 minutes.

33 Next, we are going to verify that the part is correctly and completely cut by comparing it against the CAD model. Select the compare button. Doing so highlights the areas not machined in blue. In this case the right hand side (as we know we didn’t machine this) and also the bottom of the left side, this is because the cutter didn’t pass the bottom of the block. In effect it’s showing a burr.

34 Post Processing Creating code for the CNC machines
We have so far created a list of commands which describe how to machine the part, this is not something we can transfer to the machine. To do this we post process the commands and create code for whatever machine we are running the part on. Highlight the job (or select all the processes requiring outputting) and select Post Process from the command bar. Give our program a name (I’d suggest group number and description) In the project folder the post for the XYZ is in the post folder, If we wished to output to the Denford, we could navigate to that folder containing it. Hit Post to output

35 Verifying the code Using HSM Edit and Backplot
After successful output, HSM will open the code in an editor, this allows us to verify the code is correct. Select Backplot from the menu. Play the code using the radio buttons. The program will show the centre line path the cutter will take. If all looks correct then… WE ARE DONE! Select Backplot window to open the graphics window

36 Done? Not quite! Creating a Setup Sheet
So we have our code ready to put into the machine, but how do we know where the datum is, what tooling to use, even which way in the vice the part is located? We need some set up info. From Solidworks, highlight the job and select Setup Sheet from the command line. This will create a HTML file with all of the relevant information. This can be printed for referral when setting the machine.


Download ppt "CNC machining for D&MT:"

Similar presentations


Ads by Google