2D Contour - angled multiple depth

[Anonymous]

Hey

As always I'm here when I'm in need some help. I'm using angled step down with 2d contour and problem begins when i'm not able to position cutter. Setting sideways compensation won't change side properly. End mill is always wrong side of the contour considering direction of angle. Setting compensation chooses which way end mill cuts, yet angled step down is always on the wrong side of contour. How to fix this error.

Also there is no way to use angled step down with chamfer end mill which is my main purpose.

Pictures: http://imgur.com/a/DQSNc

Need solution ASAP. I hope i'm not making some kind of stupid mistake myself.

Best regards.

[daniel_lyall]

Click on the red arrow when you are in the geometry tab, and please post the pick in your post most people will not go near a external link.

[Anonymous]

Changing correction parameter wont help. Changing contour direction, with red arrow, won't help either.

Using 2d chamfer tool path won't give step down menu as 2d contour with chamfer tool.

First picture condition with chamfer mill other side contour is what i need. Then the step down angle is correct.

Best regards!

[daniel_lyall]

Can you post your model, Go to File -> Export and save as a .F3D Archive File and attach it to your next post

[Anonymous]

Hi

There is no need to send fixture assembly because on part level same behavior happens. Customer is waiting and getting anxious. This problem has taken couple of days for me.. 

Also is there any way to use same step down behavior with chamfer mill?

It seems I found bug. When I select bottom plane then 2d contour makes this weird behaviour. If I offset from selected cutting contour step down works.

But this wont help me either.. I need to use chamfer mill. 2d contour and 3d won't support camfer milling angled step down. Is this even possible with fusion360?

File is in the attachments

Best regards

[daniel_lyall]

A 3D contour does it with no problems.

You made a few big mistakes, The setup was not done correctly, you need to set the model orientation and pick the body in the setup.

A 2D toolpath for something like that is the wrong toolpath to use.

I have added a 2nd toolpath what will cut both sides only.

Your file attached for references. 

[Anonymous]

Thanks in advance! I will check this when I get to my cad station. 

Best regards!

[Anonymous]

My take on this:

2d contour works without problem if you create "bottom plane" offsetting from selected contour. If  bottom plane is selected using body or other references then Fusion can't handle situation. Selected contour has to be open. 

I am considering it as a bug if i get two different solutions but should get same results.

.. if you create "bottom plane" offsetting from selected contour... 

To daniel_lyall -  Your 2D contour wasn't working properly. Your tool path runs through main body. 3D contour was okey.

Now if I want to use chamfer mill whit configured settings and select it I get error.

Is this even possible with fusion? Customer is waiting and if Fusion isn't capable doing this I'm forced to consider my buddys mastercam license.

Also why would you consider next thing?

A 2D toolpath for something like that is the wrong toolpath to use  -  I would say it's normal tool path because all contours, even tho they are projected in 3d space, will be 2d contours in the end.

You made a few big mistakes, The setup was not done correctly, you need to set the model orientation and pick the body in the setup - Yes here you are right jet these conditions won't actually affect at this case. If I'm re-contouring your 2D toolpath with same open contour. Same thing occurs if bottom plane is selected not offset.

So my main question here is -  Is this stepped down chamfer mill possible with fusion?

Best regards!

[cj.abraham]

It appears this is an oversight for using chamfer tools with 2D contour. A ticket will be created to support multiple depths in 2D Contour with a chamfer tool.

In the mean time, the workaround is to define a tapered endmill that is the dimensional equivalent of the chamfer tool, and proceed with the 2D contour at an angle.

[daniel_lyall]

@Anonymous That's just the way I would do it useing a 3D contour, It's easy and quick to set up. It was just patch pick the toolpath pick the body and patch set an angle so it only hits the angled surfaces done.

You get use to what does and does not work, most people if they say they are in a rush, like the quick and easy toolpath that just works as it should.

[eschermuppet]

@cj.abraham  I Just found this suggestion, and it's been helpful, but raises another question.  Does anyone know of a way to reverse the stepdown (or, I guess in this case it would be called a stepup). I'd rather not risk the point on my chamfer mill unnecessarily by having it participate in milling the stock, but can't figure out how to get it to start at the bottom of the contour and work its way up along the incline. 

[jbthornhill]

This would be a very helpful addition at this point!

[cj.abraham]

There is not an option to order from bottom to top, but what you can do is create a 2D contour with a single pass at the bottom then use a linear pattern along the angled edge to add "passes." 

[jbthornhill]

I forgot to reply to this before, but thanks very much for this solution. Worked perfectly.

[rengfx]

Has this been implemented yet? I am currently working with a 2D contour path for chamfer mills, that call for multiple axial depths, and would be GREAT if when a chamfer tool is selected I can specify the stepdown, like I can with ANY other 2D contour instead of duplicating the pass and making custom Stock to Leave values

This is how I deal with corner radius tools and would love the functionality expanded into all 2D contours not restricted from chamfers