Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Porting tool Drills deeper than expected(Possible Bug)

7 REPLIES 7
Reply
Message 1 of 8
CuttingEdgeManufacturing
172 Views, 7 Replies

Porting tool Drills deeper than expected(Possible Bug)

Hello,

 

I have created a form tool for my porting tool, and i physically measured from tip of the tool to the spotface diameter, and added the amount needed for the spotface. comes out to .900"~.

 

however in the posted code it is much deeper. resulting in a scrapped part. no matter how much i look at this i cant seem to figure out why its doing this. 

 

My best guess is that it pertains to the form tool creation in F360, whether its me not setting it up right or possible just some weird quirk.

 

regardless here is some screenshots and also a f3d file. this is possibly a bug.

 

in the below photos T19 is what is in question.

 

Screenshot_207.pngScreenshot_206.pngScreenshot_205.png

7 REPLIES 7
Message 2 of 8

Zmin equals your tip offset value -.910 and your bottom height offset -.285, so the issue is likely somewhere in those two. 

 

Where are you touching off the form tool? If it is on the tip you do not need a tip offset. Then set your bottom height to the depth you want the tool to go. 

Message 3 of 8

-.285 + -.91 = -1.195

Program the drill Op as Origin -.91 for the port tool, but according to your sketch/model it should be -.64 for the tool and -.2 from your cbore.

z-.84 is the right thing to program then comp at the machine. 

Please click "Accept Solution" if what I wrote solved your issue!
Message 4 of 8

my tool was set to the tip. just like a normal drill. i set my depth to -.9 which is how deep i want to go. however it went much deeper.

Message 5 of 8

why would i ever want to comp a drill at the machine? from the point of the tool is where the tool is set. i want to type in -.9 from model top and it go down .9 just like any other drill?

 

why isnt this doing exactly that?

Message 6 of 8

@CuttingEdgeManufacturing you mention the T19 port tool, but what about T16 (also a SAE port tool), is that one behaving correctly? (Simulation says "no")


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 7 of 8

 

that one, bottom height is -.9", then the posted code is .9625" so yea same problem but with different amounts. not sure where that one comes up with the extra .0625 on the depth.

Message 8 of 8

Because its a port tool? In our shop, we try to avoid cutting the /32 spot face with a port tool (for some picky customers) due to a myriad of issues that can come with it VS a controlled, new 3/8 endmill. I'd also suggest threading it before using the port tool - it removes any burr that pops up into the 45* section.

As I said before, you need to just program from Origin/Top Of Model -.9 and use that setting if you want that to happen. You have a bottom height set of -.285 in that toolpath, which is deeper then the modelled counterbore....

Everything is explained in my comment yesterday. 


As for T16, that one is wrong because you set your WCS off of STOCK and not PART. It's fairly evident when you know what to look for.
wrong 2.PNG

 

wrong 1.PNG




Please click "Accept Solution" if what I wrote solved your issue!

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums