operation - parallel

[Anonymous]

Hi

I have a questions. In my toolpath file I put the parallel operation. The geometry which is operated is the part of the plastic injection mold. What parameter controls the course of the optimization path  for unnecessary runs - those  runs which are shown in attached image? This is the beginning of the path, and then the tool enters deeper into the stock and after all is OK.

Ludwika

[bobvdd]

Ludwika,

Have you tried using the Machining Boundary option on teh second tab (Geometry tab) to restrict the toolpath?

Other options are to use the Slope or the Top and Bottom height plane positions to restrict the toolpath.

Bob

[Anonymous]

Thanks Bob.
I will try tomorrow, now I'm waiting for update. Maybe I share you this
model with toolpath file.
Ludwika

[Anonymous]

Hi Bob.

How can I invite you to the project ,where the file is placed. I dont have your email address. I have still problem with unnecessary runs in the toolpath.

Ludwika

[bobvdd]

My email address is bob.van.der.donck@autodesk.com.

As an alternative to sharing, you could export the cam360 file by using the File > Export ... menu.

Then send me that file or post it here on the forum.

Thanks.

Bob

[Anonymous]

Hi Bob

Toolpath file is attached in email. Main operation is parallel_1 other operatrions are just for test. The problem is with these runs on the ramp surface when the tool begins to mill the cylindrical surface. I dont want these runs . Theoretically, they can be avoided by dividing the operation into three sub-operations :

first - above flat surface,

second - above cylindrical surface

and last above ramp surface

But this not good solution , tool will working in contact with  a large vertical surface. So will problem with a stress in the material , in the tool , that can generate deformation in created forms.  And of course a lot of unnecessary heat

Ludwika

[bobvdd]

I think you need to set the contact point boundary checkbox on.

This option is specifically intended to avoid the border overlap that you were concerned about.

You also have set your additional offset to 1 mm, I think it is better to set that back to its default value of 0 as well.

[Anonymous]

I made these changes, but they do not affect the path.

Please look at the picture I attached. 

Why the tool after reaching point A does not return to milling. All runs up point A are unnecessary. I would like to avoid the milling of the air.

[jeff.walters]

Is it possible that you have a surface that is hidden?

[bobvdd]

I suspect Ludwika simply selected a too broad boundary. In order to restrict the toolpath to the slanted face, a smaller boundary is necessary.

And that boundary can only be obtained after editing the selection. See this video.

[jeff.walters]

Yes but having too big of an area would have caused the tool to cut along the flat top. His screen shot looks like it is continuing to cut the angle up and out of the stock well above the part. Unless we have a major bug here the only way I can see that happening is if there is a surface or other part that is hidden.

[Anonymous]

---

@jeff.walters wrote:

Is it possible that you have a surface that is hidden?

---

Hi Jeff 

There is no hidden surface. The body is made by combine operation

Ludwika

[bobvdd]

So my last video did not solve your problem? 

[Anonymous]

---

@bobvdd wrote:

I suspect Ludwika simply selected a too broad boundary. In order to restrict the toolpath to the slanted face, a smaller boundary is necessary.

And that boundary can only be obtained after editing the selection. See this video.

---

Hi Bob

Firstly , excuse me , real precision of expression is the  first of all. So we are at the beginning of the problem. The boundary selected is the smallest of the selected. In this moment I have no idea what to do . I will try with split operation in the weekend.

Have a nice weekend!

Ludwika

[Anonymous]

Hi Bob

The problem of milling air is solved. It is importrant to good set value maximum stepdown and value number stepdowns. I had first 4 mm and second 20 ,it was wrong.

But another problem appeared. Now I have set Tool outside boundary and Additional offset 4  mm ( the tool has 6 mm diameter) . The prompt informs that is horizontal offset , OK this horizontal offset but on the bottom height , the tool is falls on the wall of the stock and move for 4 mm ( from the wall of the stock ) , on the bottom height. The offset bottom height is specially set to 20 mm

All stock offsets are 0 mmm .The questions are :

1. Why does the tool fall to the bottom height when Tool outside boundary is set ?

2.Why is offset implemented on the bottom height ?

By me offset should be implemented on the  current mill surface.

Bob be so kind and check my model,  maybe somewhere my settings are wrong again.

Many thanks for your support.

Ludwika

[bobvdd]

Ludwika,

I saved a new version of your part.

In Parallel1 operation, I changed the bottom plane to be flush with the top horizontal face of the part rather than 20 mm offset.

I kept Tool outside boundary and I also kept the additional offset of 4mm.

Here is a side view of the resulting toolpath. Is that what you were hoping to get?

[Anonymous]

Hi Bob
It looks perfectly for flat surface. Conclusion is that the strategy
*Paralle*l or *Horizontal* with *Tool outside boundary* is proper for flat
surface. For the ramp or cylindrical surface must be applied the other one.
I was looking for but still have not found good.
In all other I have unnecessary runs , I don't why tool falls always
to the *Bottom
height*. The best looks *Pocket* with* Tool center on boundary*. I think
this will be used .
Ludwika

[bobvdd]

Ludwika,

I can perfectly use Parallel for non-flat surfaces. Parallel is certainly not restricted to flat surfaces.

Here is an example where I use a Parallel with following settings

Tool center on boundary

Additional offset = 0

Bottom height plane at the bottom of the part.

And you can see that the toolpath is nicely contained.

It does not overspill on the sides and it does not go all the way down to the bottom plane either.

Bob

[Anonymous]

Hi

It looks nice, but when I changed tool - flat mill 22 mm diam. instead ball mill and angle for 0 deg please look what happened.

The ball mill is the finishing tool , in the first step model should be treated roughly by flat mill. This operation must be carried out with Tool outside boundary option which in this case is cumbersome.

Offset for this option should be other than 0 , the best if it is more than half of tool's diameter. The errors shown on the picture are caused by the lack of offset. The flat mill should works by the lateral surface, but not bottom face. I think that the algorithm of the pararell strategy has an error because it does not detect collision in this moment .

Thanks for your patience with me.

Ludwika

[jeff.walters]

I noticed that the operation has a warning on it. What does the log file say?