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
Solved! Go to Solution.
Solved by bobvdd. Go to Solution.
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
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
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
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 :
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.
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.
Is it possible that you have a surface that is hidden?
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.
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.
@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 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
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
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?
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
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
I noticed that the operation has a warning on it. What does the log file say?
Can't find what you're looking for? Ask the community or share your knowledge.