I was using the hole machining operation in Sprutcam to machine some large diameter holes in a 2" thick piece of 6061 yesterday using a 1/2" dia. 2" flute endmill.

I quickly found out that the feedrate I had set for milling was way too fast for plunging during each step.

I looked in the parameters settings and tool settings in Sprutcam and didn't see anyway to set a different feedrate for plunge and mill.

In looking at the Tormach wizards I see that they do allow for different feedrates for the two operations but can't understand why Sprutcam doesn't.

Maybe my glasses are just bad!?

I am a fairly new Sprutcam users so this may or may not be the correct answer. From what I have read and experimented with it looks to me as if you need to use two operations. One operation will use Hole Machining to do the plunge, and then a machining type operation to actually mill the part. It sounded goofy to me but that was my take on the process.

I believe there was a post (maybe on the SprutCam forum) talking about a similar issue. I think someone from that post forwarded a request to SC for an improvement in a future version of software.

I will be trying something like this shortly so if you find an answer please let us know the solution.

Robert

RTP_Burnsville,

Thanks for your reply.

I was thinking about a separate drilling operation also but thought that I was maybe missing the parameter setting somewhere and a simple click would solver the problem. (it wouldn't be the first time) Besides drilling (or machining) the plunge hole first would waste some time during the plunge part of the pocketing step as it would just be cutting air.

I have a hard time believing that they just missed it when designing the software as there are parameters for just about everything else. As I mentioned, the wizards I looked at had separate plunge and mill parameters.

Your right though... I think it is something that could easily be added in a revision.

I manually edited the NC file to change the feedrate before and after each plunge as I didn't want to bother with another operation especially if I end up machining more of the same part in the future.

Guys -

It seems that I always end up editing my programs for things like that, too. You can fix it in SprutCAM before you post by editing or adding a line on the simulation page. I have removed a lot of air cutting (and SprutCAM mistakes) that way, and it does work. Just don't rerun that toolpath or you'll loose your edits. You'll also loose edits if you repost over an edited program, of course.

You could try setting the maximum plunge angle to 15 degrees or so (on the tool page) and let SprutCAM ramp into your pocket instead. I have not tried this, but have considered it a few times. I should start using it, but I'm too lazy to change my habits. Besides, those plunges are always so fast, they're exciting...

I think that if you really wanted a plunge, the hole drill operation would be a good solution. You can specify the same endmill, and SprutCAM won't generate a toolchange. It would just plunge at the rate you specify to the depth you specify, then use that hole for the faster plunges later during the pocket cutting.

Heck, if you haven't snapped a mill off during a plunge, you could just leave it like it is...

Regards,

- Just Gary

I normally hate making manual edits because if I make a change to the part or one of the parameters for the machining operation later on (and have to re-post the program) then I need to have to repeat all of the manual edits again. With my short memory I usually end up forgetting exactly what I did the first time.

The thing that made these plunges especially exciting was that I had two 5/8" clamping screw holes equally spaced (1/2" on each side of center) of the circular pocket (from previous operations) so the endmill wasn't totally contained as it plunged. I thought for sure that the CNC was going to jump off the stand even though it is bolted to it. To add to the excitement... I was using a brand new ($140.00) 1/2" carbide 2" LOC bullnose endmill.

I didn't think about the plunge angle setting as I wasn't quite sure what it did. Does it bring the tool into the workpiece at an angle to the top surface by moving all 3 axes simultaneously? Or is it for something different?

Why not use a waterline operation and adjust the plunge speed in the feedrate tab?

Thats what I do.

David

I don't know if it is available in all ops, but there is a drop down list in the Feedrate tab where various feedrates can be set. It looks like the one labeled "Approach" is the same as the plunge rate. Have you seen that yet?

Mike

I already checked. That particular machining operation only has Rapid, Work and Return feedrates which is surprising because you would think that plunge rate would be important.