Back chamfer - how to?

[scotS3G9D]

I found an older article about creating a form tool and how to program a simple back chamfer but it's not working.  It's not entirely clear to me if you're to use the 2d chamfer or 2d contour options.  I have my form tool set up but can't figure out what to do next.  Can someone help?  This is the article I found:

https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/simplecontent/content/undercutt...

Thanks, Scot

[GeorgeRoberts]

Hello

I usually use 2D contour for this. Please see the attached file as an example. If you check the expressions in stock-to-leave, you will see the formulas that are shown in the article.

Be aware, this is prone to colliding with the model, so ensure you check carefully and simulate prior to running on a machine

[scotS3G9D]

Thank you but I'm having trouble opening the file.  I needed to update Fusion and restart but it still won't open.  I've attached a log file.

[csl1016]

https://youtu.be/g9FV0n4PsvQ

[seth.madore]

That's because the file was saved in a Developer build of Fusion. Since it's "from the future", it can't be opened in Production. Tsk Tsk..

So, here's the formulas you want to use in your Stock to Leave settings:

Radial:

if (abc.isNonZero()) {

      gRotationModal.reset();

      writeBlock(gRotationModal.format(68.2), "X" + xyzFormat.format(0), "Y" + xyzFormat.format(0), "Z" + xyzFormat.format(0), "I" + abcFormat.format(abc.x), "J" + abcFormat.format(abc.y), "K" + abcFormat.format(abc.z)); // set frame

      if (true) { (!isPrepositioned || !section.isMultiAxis())

        writeBlock(gFormat.format(53.1)); // turn machine if not prepositioning for a multi-axis move

      }

Axial:

-((tool_diameter-tool_tipDiameter)/2*Math.tan((90-tool_taperAngle) * Math.PI/180))+(chamferWidth*Math.tan((90-tool_taperAngle) * Math.PI/180))

So, how do you enter those? Go down to "Stock To Leave", turn it on and then click on the three-dot icon to the right. Select "Edit User Expression". This opens a new dialog box, so just copy/paste those values

I'd suggest that once you have that done, then create a Template of "Back-Deburring"

[scotS3G9D]

Goodness...I have no idea what all that means!  The radial formula says invalid expression when I try to use it.  The axial formula was okay.  When using this in 2d contour, how would you adjust the chamfer width?  I'm assuming you use 2d contour?

[scotS3G9D]

Thank you for your video.  It's hard for me to follow but I think there's some practical info hiding within it.  Practical meaning it might be something I could comprehend but it's a bit of a language challenge.

[scotS3G9D]

Hi Seth,
Can you confirm the radial offset formula is correct?  It makes no sense to me when I look at it and it's not working.

Thanks, Scot

[seth.madore · Accepted solution]

Radial:

(tool_diameter-tool_tipDiameter)/2-chamferWidth-2*(chamferTipOffset/Math.tan((90-tool_taperAngle) * Math.PI/180))

Axial:

-((tool_diameter-tool_tipDiameter)/2*Math.tan((90-tool_taperAngle) * Math.PI/180))+(chamferWidth*Math.tan((90-tool_taperAngle) * Math.PI/180))

[scotS3G9D]

Thanks, Seth.  I can't figure out why I don't have the option to set a chamfer width in 2d contour.  A recent update seems to have removed that ability for me.  

[seth.madore]

---

@scotS3G9D wrote:

Thanks, Seth.  I can't figure out why I don't have the option to set a chamfer width in 2d contour.  A recent update seems to have removed that ability for me.  

---

You do have a Chamfer tool selected, right....?

[scotS3G9D]

Ah, actually no.  I made a form tool.  I tried something beforehand and it didn't work so thought I needed a special tool.  Let me try it again.

[petermorphett]

Why doesn't this option have lead to centre, if your using a back chamfer tool that is close to the hole size, it crashes in to the sides of the job on the way out and you have to fudge the lead in and out settings..

Is there a expression to add so it adds lead to centre no matter what the to OD of the tool is?

[programming2C78B]

old mastercam trick here = yes!

It will be slightly off since the tool "dia" is where it makes contact with your hole feature, not the true OD of your chamfer tool (this expression is made for endmills interpolating). You can also try using Drill Points and Keep Tool down.

I keep an excel sheet with all of these. Hope it helps! 

[petermorphett]

So where are you plugging in this value?

[programming2C78B]

thats your horizontal lead in length and radius with a 135* sweep angle 

Last tab, leads and transitions.