Need Help!- Indexing on the 4th axis

[bevinp]

I have a simple task to machine a pentagonal head on a screw by using the rotary table as the indexer. The rotary table axis will be parallel to the X axis and the workpiece held in the chuck. Each face of the head will be engraved with a number. See atttached project.

I have spent some hours trying to machine the pentagonal head with only 80% success.

SC 7 Help info is good but incomplete (I think):
"In SprutCAM you can easily set the rotary axes position by clicking on the part face which the tool axis has to be aligned to. This method is performed with the following steps:

1. In the operation Setup panel select the <Rotary axis> parameter and press the ellipses button at the right of the caption. The <Align Tool> dialog will appear.
2. To align the tool with regard to a flat or a cylindrical surface just click on that surface in the graphic view.
3. Press <Ok> to apply the changes.".

And

"... set the parameter <Local coordinate system> to the <Auto> mode."

However,I have not found the machining operation that works well. Most end up with weird tool paths that don't follow the Parameter bottom and top settings.
Help.
Bevin

[Live]

Originally Posted by bevinp See atttached project

Hello Bevin, Where is the project?

[bevinp]

I thought I had sent the attachment, Let me try again.
bevin

[bevinp]

Hopefully it is attached now
Bevin

[Eric_Tormach]

Bevin, attached is one way of doing this job, however it seems as if the model might be off center. This way I used 2D contouring with "multiply toolpath by axis" in the transformation tab in the parameters box. Another way of doing this would be to use the flat land finishing operation that you have done. Copy and paste that operation so you have five total. Then using the setup settings set the first operation to the A axis value of 0 and for each subsequent operation add 72 degrees to the A axis value.

[bevinp]

Eric,
Thanks for the response.
The file that you attached perhaps was the wrong file.... the operations it had were Flat land finishing and not 2D contouring. As I suspect you know, Flat land seems to fail after the first indexing. It seems to be a bug with SC; do you agree?

As you say, I could copy and paste the flat land routine to manually get the Gcode file, but that would be giving up.

I tried the 2D contouring with "multiply toolpath by axis" but could not get it to work but apparently you have. So please explain the settings you used (or send me the project).

Bevin

I

[Live]

Originally Posted by bevinp Eric, Thanks for the response. The file that you attached perhaps was the wrong file.... the operations it had were Flat land finishing and not 2D contouring. As I suspect you know, Flat land seems to fail after the first indexing. It seems to be a bug with SC; do you agree? As you say, I could copy and paste the flat land routine to manually get the Gcode file, but that would be giving up. I tried the 2D contouring with "multiply toolpath by axis" but could not get it to work but apparently you have. So please explain the settings you used (or send me the project). Bevin I

Hello Bevin.
I've investigated your project and found out why the
flat land finishing operation does not generate any toolpath.

The reason is simple. The operation accepts only those flat faces,
whose Z level is between the Top and Bottom levels you specify in
the Parameters panel. Just open the parameters panel and uncheck the
Top and Bottom level options.

The second problem is the part is not properly set up in the workpiece holder.
It is not centered. That's why the "multiply toolpath by axis" feature does not work properly.

The third problem is the part is inversed by some reason. Go to the 3d Model tab, select any face of the part, right click on it and select the Inverse command from the 3D Model popup menu.

I'll attach the modified project.

[Live]

Originally Posted by Live Hello Bevin. I've investigated your project and found out why the flat land finishing operation does not generate any toolpath. The reason is simple. The operation accepts only those flat faces, whose Z level is between the Top and Bottom levels you specify in the Parameters panel. Just open the parameters panel and uncheck the Top and Bottom level options. The second problem is the part is not properly set up in the workpiece holder. It is not centered. That's why the "multiply toolpath by axis" feature does not work properly. The third problem is the part is inversed by some reason. Go to the 3d Model tab, select any face of the part, right click on it and select the Inverse command from the 3D Model popup menu. I'll attach the modified project.

Here it is.

[bevinp]

Thanks Live,
Unfortunately I was not able to open the attachment... message displayed said ".. version not supported", so I guess my SC7.0.6 is too far behind yours.

I attempted to download the latest 7.1 version from SC RU website but download failed after 85KB on three attempts. I have emailed SC for assistance.

I then followed your advice. I did know about the need to recentre the X axis on the centreline of the part and admit to inverting the model when I was following older indexing advice, SC2007, from CNC website (and then forgetting it). After unticking the top and bottom boxes the Flat Land Finishing work fine, except for the toolpath between the 4th face and the 5th face. The rotary movement was a full 360 then plus the last 72 degrees. So far I haven't been able to correct that. Any thoughts?

The Flat Land Finishing toolpath tracks the centreline of the tool over the outer edges of the flat surface, rather than just running down the centreline of the surface and therefore maching the surface in one pass. I am going to try other machining operations. Any comments?

I did not have time today to try the 2D Contouring with the multiply toolpath technique, will do tomorrow.

Thanks once again Live,
Bevin

[bevinp]

Hi Live,
I eventually updated my SC to 7.1 and now can view your attached file. I am surprised at how few settings are needed to multiply-by-axis.

But I haven't experimented with other operations yet because my updated SC immediately closes down whenever I select Create (a new operation) in the Machining tab. I am working on fixing that problem at present.

Bevin