topic Re: Help with first thread milling job using Fusion 360 in Fusion Manufacture Forum

Help with first thread milling job using Fusion 360

jgaertner — Sat, 09 Jun 2018 20:06:06 GMT

Hello Forum,

I have a project that I want to use single point thread milling on to machine an external thread in a gauge face plate we make. I am using a lakeshore Carbide single point .30" thread Mill.

http://www.lakeshorecarbide.com/38singleprofilethreadmill34loc300cutdia14-40range.aspx

I have set the mill to make three passes of equal depth. The pitch diameter offset is stated as 0.02255 in Machinery's Handbook. I would like to get some confirmation from other Fusion users that I am approaching this correctly? I need 24 TPI on the outside of the gauge flange. I would appreciate any constructive assistance.

Thanks,

Jgaertner

Re: Help with first thread milling job using Fusion 360

jgaertner — Sat, 09 Jun 2018 21:11:11 GMT

I wish to make some changes on this post I made. I am attaching a new file. I think I had the Diameter Offset off.

Jgaertner

Re: Help with first thread milling job using Fusion 360

Steinwerks — Sun, 10 Jun 2018 15:57:51 GMT

Before I dig too far, is there a reason you're not using the Thread Mill tool type? This would give you a much more accurate representation of the result.

Re: Help with first thread milling job using Fusion 360

jgaertner — Sun, 10 Jun 2018 16:41:21 GMT

Hello Neil,

Thanks for that help! I did not scroll down far enough in the tools to see there even was a single point threading tool. I know a request for one had come up on the earlier posts that I read on line before making this post. I have attached an updated file. I do not have the tool in my shop yet, so the details may be a little bit off...

Jgaertner

Re: Help with first thread milling job using Fusion 360

Steinwerks — Sun, 10 Jun 2018 18:59:28 GMT

In terms of the tool's thread pitch you want to give it the maximum thread of which it is capable, so in this case I simply divided one by 14 to get 0.0714286. You can input this directly into the pitch field as 1/14 and it will calculate for you. This results in a (close to) correct shank diameter (which is helpful for clearance checks). You can add a shank section to represent the transition from shank diameter to shaft diameter. Not very important for shallow operations but always a good idea to represent the tool as accurately as possible IMO.

For thread milling I would recommend Wear compensation (or In Control if that's your thing). Nothing is more irritating than having to repost the same program with slightly smaller offsets many time in a row. This way you can start large and work towards the correct diameter offset.

FWIW I have never had much luck with thread milling in HSM, and found it to be a lot of trial and error. Once I find the correct offset at the machine I modify it in the CAM and repost.

I have had better luck with OD threads though than ID threads, modeled at the minor diameter with no thread offset, usually within about .005" of nominal.

Re: Help with first thread milling job using Fusion 360

M>oolWorks — Mon, 11 Jun 2018 02:31:43 GMT

To echo Steinwerks I have not had the best success with fusion and thread milling off the bat. It took a fair bit of tweaking to get it dialed in and it seems to vary slightly between jobs. I cannot quantify WHAT is different, but one job might be spot on, the next .003 off, then next .001, the next spot on. I do not think it is my machine, but something with how the helical interpolation is done with the pitch geometry. Not really an issue for a bigger job, but irritating for one piece.

The good news is that the error seems to consistent. So as Steinwerks mentioned, setup your piece, thread mill it to the correct pitch diameter, then offset your settings in Fusion, so that the next time it is posted, it is correct.