The plan was quite simple.

Cut a turned part to be machined on both sides from the bar and at the same time programme the second machining side. If the length of the blank is defined to such an extent that at the end, there is enough material to “cut” out of the protective zone for the chuck or the clamping jaws.

However, if you proceed as described, after the “cutting off” step it would result in the half-finished workpiece falling in the simulation as in reality the chip tray or a part catcher. Afterwards, the geometry is no longer available in the working plan for further machining.

But what is the solution then? The following practical tip gives you the answer:

Step 1: 

Instead of giving the blank an excessive length, make it only slightly longer than the finished part and assign negative values to the outer and inner values of the protection zone (tool width of the parting line).

Step 2: 

The half-machined workpiece (red lines) then remains in the routing and can be saved in this form via F1 “File” > F7 “Export” > F1 “Workpiece geometry”.

Step 3:

The new blank can then be used for a second working plan.

Step 4:

Under F4 “Clamping” the workpiece is first turned over. Special attention must then be paid to the input field “Shift Z”. In the example, -0.4 must be entered because, in addition to the stock allowance for the second side of 0.2 mm here, the “slug” left by the cutting radius of the parting-off tool must also be taken into account.

Step 5:

The last step is to determine the work steps as usual and as on the first page. Here you benefit from the so-called contour tracking of the software, which recognises where drilling and roughing has already been done from the first page. This becomes visible when creating the work steps by the correspondingly reduced red areas (here for the roughing cut inside).

Now it’s your turn.

Was this tip helpful? Let us know.

You will find more tips in the upcoming newsletters.

You have questions? Contact our experts using the contact form below.

Working with islands (or tenons) can get complicated.  However, with SYMplus™ this task is quite easy.

And this is how easy it is:

You want to manufacture the following workpiece and for this purpose you first create it in the “Geometry” operating mode.

This workpiece is composed as follows:

1. From a rectangle on the depth -10 
2. On it an island (light gray) with the depth 0
3. A “bitten” rectangular pocket in the islands at depth -5 (however, this pocket must also be constructed like the light gray surface with 6 lines and then 4 curves, so that the contours are partly on top of each other). 

In SYMplus™ we understand the depth/height of the surface not as the traverse depth of the tool but as the depth or height of the surface circumscribed by the contour. It is important that each contour is closed. To check whether you have done everything correctly, you can look at the 3D image of the workpiece.

When you have created and saved the workpiece, switch to the ” Work plan” operating mode. There you first edit the rectangle at depth -10. 

If you use the preset cutting type “Contour parallel” when creating the working step on the third dialog page, you will notice that the milling cutter makes full traverse paths and then only clears out the material with the set pressure width.

To prevent this, change over to “Tenon” for surface milling by one island.

Since the island has a narrowing (or “port entrance”), a working step must also be created for this. To do this, as with a pocket, clear out with the machining type “Contour parallel”.

In the ” Work plan” you can easily try out alternatives to this machining strategy by undoing the work step and creating a new one. For example, you can place a groove in this narrowing and first machine it trochoidally.

Now it’s your turn. Try it out and see for yourself how easy it is to handle islands and tenons with your SYMplus™ software.

You will find more tips in the upcoming newsletters.

You have questions? Contact our experts using the contact form below.

Thanks to SYMplus™, many things work automatically. The programming of the traverse paths, e.g. in the case of roughing, is normally simply removed from your hands. Sometimes, however, it can happen that the automatic system reacts differently than the expert imagines.

This can happen if, for example, you need to traverse a very special path with a special tool.

For this SYMplus™ offers a very simple solution. And it is called: “Handwheel”.

If you depend on it, you can create this work step in the operation mode ” Work plan” just as uncomplicated as any other work step. Specifically via F1 “Create” and F6 to select the “Handwheel” afterwards.

Step 1: 

As described before, create a new work step with F1 and then select the “Handwheel” with F6.

Step 2: 

Next, press F2 “Manual”. This will activate the “Manual Positioning”.

Step 3:

Then manually move to the Z value 1,000.

This works as follows:

3.1 Shift+F6 selects the 3rd decimal place. Press the “+” key on your keyboard to set the value to 0.

3.2 The 2nd decimal place is selected with Shift+F5 and again you have to use the “+” key afterwards.

3.3 The last digit to be selected is the 1st decimal place. To “jump” to this digit, press Shift+F5 again and then use the “+” key to finally set the value to 1,000.

Step 4:

After this setting of the Z-value, accept it with F10 “End input”.

Step 5:

Now we want to move to the tool change point. To do this, select F1 “Position” and change the setpoint to X = 150 and Y = 150.

Step 6:

 Switch to rapid traverse with F7 and then confirm the entry with F10.

Step 7:

Press F10 a second time to return to the “Handwheel dialog”. Then press F10 a third time to accept your new “Handwheel” work step.

You will find more tips in the upcoming newsletters.

You have questions? Contact our experts using the contact form below.