[MetalShavings]

I spent about an hour and a half today trying to generate some High-Speed tool paths with my version 7 SprutCam. No matter what combination of inputs I tried I just couldn't get what I was looking for. It seemed like the closest I could come to the right High-Speed tool paths ended up with my end mill mowing down the features I was trying to machine.

I could get my end mill to make the cuts with the side of the tool but, it wouldn't cut around the features I was trying to shapet in the first place. I'm sure it's not that hard for someone who knows what they are doing with this CAM software. I guess I'm just not that person; not yet anyway.

I've viewed the video tutorial posted above on the HSM-ing of a slot but my project isn't a slot so I can't quite use the same perimeters. Does anyone else know of any video tutorials that can shed some light on this subject using SprutCam? I really would like to get this HSM thing to work for me.

MetalShavings

[bevinp]

metalshavings,
I am not sure I understand exactly what you have tried, so let me begin at the top and I apologise if I seem to be patronising you.
High Speed Machining is essentially using the side of the cutter and therefore the Depth of Cut (DOC) is the measurement along the axis of the cutter, usually being the full Z thickness of the part, but only using very small Width of Cut (WOC) which is the radial depth of cut.
In SC7-> Machining -> Finishing ->2D Contouring-> Create. Double click on the 2D Contouring operation. Select tool.
Under Feeds/Speeds, select those values as per your Speeds and Feeds Calculator. The Feed for HSM is much faster than when cutting with 1/4 or 1/2 diameter of the cutter. Also usual style is climb milling.

Under Lead in/out, enter your choices but usually arc or tangent path out..
Under Parameters, set the DOC to the thickness of the part or the maximum axial length you can machine in the Z direction.
Under Strategy this is where the HSM settings are user specified. In the “Rough step parameters” window, tick “Roughing XY paths” box, in “Zone width”, enter the maximum thickness of the workpiece that has to be machined to achieve finish part size in the X and Y planes, For “Step” enter the axial width of cut WOC that either you specified for your S$F calculator or which your calculator provided.
It would be appropriate that the entered WOC allows for chip thinning but if you are unsure of this consideration then tell us what exactly your workpiece/part sizes are and we can give you advice. SC will auto calculate the number of steps will be coded.
In Finishing parameters window, you can specify what finishing WOC cut you believe will be necessary to improve the finish or the accuracy of the part.
Under Transition, you can decide whether to have the tool high speed motion between cuts to be either above the workpiece of around the workpiece.

Good luck
Bevin

[wtopace]

I spent about an hour and a half today trying to generate some High-Speed tool paths with my version 7 SprutCam. No matter what combination of inputs I tried I just couldn't get what I was looking for. It seemed like the closest I could come to the right High-Speed tool paths ended up with my end mill mowing down the features I was trying to machine.

I could get my end mill to make the cuts with the side of the tool but, it wouldn't cut around the features I was trying to shapet in the first place. I'm sure it's not that hard for someone who knows what they are doing with this CAM software. I guess I'm just not that person; not yet anyway.

I've viewed the video tutorial posted above on the HSM-ing of a slot but my project isn't a slot so I can't quite use the same perimeters. Does anyone else know of any video tutorials that can shed some light on this subject using SprutCam? I really would like to get this HSM thing to work for me.

MetalShavings

bevinp has some good suggestions below, but if you're still a little confused, feel free to shoot me a PM for my email address. I'm definitely not a Sprutcam expert, but I have produced quite a few complex parts with it. I would be happy to take your stc file or part file and create some toolpaths for you and send it back. I'm running Sprut9, so I'm not sure how well it interoperates with Sprut7, but it's worth a try if you would like a little help.

We all need help from time to time, MountainDew used to post quite a bit here and has helped me a lot in the past via email when I was in a bind, so I have quite a bit of debt to repay to the community =)

Here is another really good HSM video - Everything from Sol has always been excellent in my books

https://www.youtube.com/watch?v=ABtsuglGrMY

[bevinp]

metalshavings,
Re-reading your posts, are you having problems selecting the edges and surfaces to be machined (called Job Assignment) or selecting the appropriate Machining operation?
Bevin

[MetalShavings]

metalshavings,
Re-reading your posts, are you having problems selecting the edges and surfaces to be machined (called Job Assignment) or selecting the appropriate Machining operation?
Bevin

I'm not having a problem with either of those two things. My problem is knowing which of the many items found on the "Strategy" page and on the "Parameters" page to click on; and having clicked on them, knowing what numbers to input in order to get the HSM results I'm wanting to get. What I'm wanting to get are High Speed tool paths that machine away all unwanted metal and leave me with the shapes I originally designed with my CAD software. I can do it with conventional milling but, if I can figure out how to do it using HSM, it will speed up the process tremendously.

MetalShavings

[bevinp]

metalshavings,
OK, perhaps if you attach your 3D model, you could get advice on how to best use SC7
Bevin.

[MetalShavings]

metalshavings,
OK, perhaps if you attach your 3D model, you could get advice on how to best use SC7
Bevin.

The 3D Model around which my original inquiry revolves is rather secretive for the time being. I've actually been selling a few to guys from the US and a couple of other countries so, I'd kind of like to keep it under wraps for now; or at least until I can firmly establish myself as the developer and maker of these specific little parts. I hope you all will bare with me on this.

I do have a project in the works in which I'll have to machine a specialized "Receiver-Wrench" to be used for re-barreling a K31 Swiss rifle. The profile of this particular rifle receiver is such that my other "Receiver-Wrenches" just will not work. It will require the milling of a one-inch thick by 4 inch-long piece of 1018 steel. It's two halves of the same size but with differing cut-outs; bottom half and top half of the wrench.

If you are willing, I can post my 3D model of this item so that you can walk me through the HSM/SprutCam7 procedure with this project part. If you can help me out with this, I may be able to carry those instructions over for use in HSMing the tiny metal parts I originally inquired about.

What Say Ye?

MetalShavings

[wtopace]

I'm sure you would get plenty of help if you wanted to post a model. If you want to protect your intellectual property, feel free to modify the model to obfuscate it before posting.

After all, we aren't offering to do your work for you, just to provide you with a relevant example to teach you how to fish =)

[MetalShavings]

I drew up a model of the "Receiver Wrench" I was referring to in my lasts post. I wasn't sure exactly what format would be best so I included the same files in the IGES and SolidWorks formats. The actual parts are only 4 inches long but I modeled it on 8" long pieces of metal stock. This is so I can allow an overhang off the edge of my vice; then turn it around and mill the other half in the same work-holding manner before cutting my metal stock into their separate halves.

Also: I took the liberty of including a mockup of the tiny steel parts I made reference to in my original post. Although this is not the actual shape of the parts, it is the same type of milling job I'm hoping to apply the HSM milling technique to; same with the "Receiver Wrench."

Both parts will be made of 1018 mild steel using a 1/2" coated carbide end mill. The inside corners of my some of my geometry are square but don't worry about not being able to get a round end mill to cut a square inside corner. I can fix that after the fact. The "Receiver Wrench" project also has holes drilled into it. Here too, I'll be drilling those holes after machining. My main concern with these parts is figuring out how to create HSM tool paths using SprutCam 7 CAM software.

I've made two other specialty "Receiver Wrenches" in the past using conventional milling methods and they came out quite good. It took a heck of a long time to mill them though and I'm hoping that by utilizing HSM tool paths that time will be reduced significantly.

Thanks in advance for your help with figuring this stuff out.

MetalShavings

[wtopace]

@MetalShavings - Sorry, I was out of town this weekend. I took a quick crack at Sprut for your fish part - since it seemed the most interesting to me.

1/4" TiCN 3-flute carbide endmill @ 5100RPM / 68 IPM with a 10% stepover (per HSMAdvisor), full 1/4" depth of cut. I left 0.005" radial stock for a 1/8" endmill to clean up for a nice surface finish. I also added spotting and drilling to get an accurate time estimate. 12:56 is Sprut's time estimate and the stepover of 10% could probably be pushed to 15% (maybe even higher) to shave more once things are well tested.

Let me know if you need some prototypes ;-) Files should be attached to this reply.

Disclaimer: This is how I would machine it. As always, YMMV.

Attachment 298098

[mountaindew]

Awesome to help but he mentioned sprut 7 before, can he open a sprut 9 file?
I find files from one sprut version to the next are not backwards compatible.
And they allow no extra versions in your possession running anyway .

[MetalShavings]

@MetalShavings - Sorry, I was out of town this weekend. I took a quick crack at Sprut for your fish part - since it seemed the most interesting to me.

1/4" TiCN 3-flute carbide endmill @ 5100RPM / 68 IPM with a 10% stepover (per HSMAdvisor), full 1/4" depth of cut. I left 0.005" radial stock for a 1/8" endmill to clean up for a nice surface finish. I also added spotting and drilling to get an accurate time estimate. 12:56 is Sprut's time estimate and the stepover of 10% could probably be pushed to 15% (maybe even higher) to shave more once things are well tested.

Let me know if you need some prototypes ;-) Files should be attached to this reply.

Disclaimer: This is how I would machine it. As always, YMMV.

Attachment 298098

Twelve Minutes; Holy Krap! It's been taking me a little over two hours or most of my Saturday mornings to finish a batch of five of these little specialty parts. (including post processing) Many thanks for your willingness to help. I'll try to open this file either tonight or tomorrow night. I'm swamped at work right now so I'm having to burn the midnight oil.

I was playing around with the "Action Wrench" file I made up and over the weekend I came as close as I've ever come to getting an HSM tool path. The bad thing is, I don't really know how the heck I did it. I must have tried entering different sets of numbers in the various fields at least a half-dozen time until I eventually got my simulations looking as though I knew what I was doing.

One of the things I wasn't sure about was which of the cutting strategies to use. "Conventional, Climb Milling" or "Both." When I clicked on either "Conventional" or "Climb" my end mill would come to the end of the cut path, then it would move up to the clearance height above the top of my part, then move to the position to begin another cutting path, then drop down to the one-inch depth and start the cut again.

When I clicked on the "Both" cutting strategy, my end mill would make back and forth sweeping cut paths of .01" deep; depending on how deep I wanted the cuts to be. On this setting, I got no rapids movements, just back and forth sweeping cuts.

I don't know if this is right or wrong but, it's the closest I've gotten to making HSM tool paths on my own. Hopefully after taking a look at how you went about working the "FishPart" file it will begin to make sense to me.

Thanks again. I'll post an update after I've had a chance to take a look at it.

MetalShavings

[wtopace]

Awesome to help but he mentioned sprut 7 before, can he open a sprut 9 file?
I find files from one sprut version to the next are not backwards compatible.
And they allow no extra versions in your possession running anyway .

Unfortunately, Sprut9 is the best I have to offer =( Haven't seen you around on the forums lately, hope all is well!

- - - Updated - - -

Twelve Minutes; Holy Krap! It's been taking me a little over two hours or most of my Saturday mornings to finish a batch of five of these little specialty parts. (including post processing) Many thanks for your willingness to help. I'll try to open this file either tonight or tomorrow night. I'm swamped at work right now so I'm having to burn the midnight oil.

I was playing around with the "Action Wrench" file I made up and over the weekend I came as close as I've ever come to getting an HSM tool path. The bad thing is, I don't really know how the heck I did it. I must have tried entering different sets of numbers in the various fields at least a half-dozen time until I eventually got my simulations looking as though I knew what I was doing.

One of the things I wasn't sure about was which of the cutting strategies to use. "Conventional, Climb Milling" or "Both." When I clicked on either "Conventional" or "Climb" my end mill would come to the end of the cut path, then it would move up to the clearance height above the top of my part, then move to the position to begin another cutting path, then drop down to the one-inch depth and start the cut again.

When I clicked on the "Both" cutting strategy, my end mill would make back and forth sweeping cut paths of .01" deep; depending on how deep I wanted the cuts to be. On this setting, I got no rapids movements, just back and forth sweeping cuts.

I don't know if this is right or wrong but, it's the closest I've gotten to making HSM tool paths on my own. Hopefully after taking a look at how you went about working the "FishPart" file it will begin to make sense to me.

Thanks again. I'll post an update after I've had a chance to take a look at it.

MetalShavings

If you aren't able to open the file, let me know and I'll screenshot the parameters tabs for you of all the operations.

[MetalShavings]

I tried opening the file last night. Unfortunately my older version of StrutCam 7 could not open it. All I got was a small window telling me that the file you sent me was "Not Supported."

Some screen shots of the settings you used would be helpful. I could compare them to the settings I've been trying that have shown the best results in my simulator window thus far.

I took a little time to play around with it some more last night. I worked on the other half of my "Action Wrench." I'm thinking I may have accidentally figured it out but the only way to tell is to take a chance on crashing some tools and ruining some parts. I think I'm going to look for a piece of Styrofoam to practice on before trying the real thing. In the mean time, checking out your screen shots could save me alot of headaches.

Thanks again.

MetalShavings

[wtopace]

I tried opening the file last night. Unfortunately my older version of StrutCam 7 could not open it. All I got was a small window telling me that the file you sent me was "Not Supported."

Some screen shots of the settings you used would be helpful. I could compare them to the settings I've been trying that have shown the best results in my simulator window thus far.

I took a little time to play around with it some more last night. I worked on the other half of my "Action Wrench." I'm thinking I may have accidentally figured it out but the only way to tell is to take a chance on crashing some tools and ruining some parts. I think I'm going to look for a piece of Styrofoam to practice on before trying the real thing. In the mean time, checking out your screen shots could save me alot of headaches.

Thanks again.

MetalShavings

Here you go, sorry about the file incompatibilities! Keep in mind that I usually play with the high-speed cuts options until I get what I want (anything except do not use is valid). Corner smoothing is also important so you don't increase the cutter load too high in corners (aka - don't bury the 1/4" cutter into a 1/4" rounded corner at 68 IPM).

Also, don't forget the checklist I posted earlier. Keep your feed rate overrides turned down at the beginning until you're comfortable that you aren't going to crash (10% rapids is fine, hand over the space bar, keep bumping your cutting feed rate as you go, maybe every 30 seconds or so and listen to the machine and the cut, you should get quieter as you get closer to 100%). Best of luck!

The best advice I can give for not crashing is ALWAYS model your fixtures, all of them. The Sprutcam simulator is really great and very very accurate, modeling your fixtures will prevent almost all crashes (you can still crash with incorrect offsets though). You'll notice I even modeled my 5" vise for the quick 10 minutes I spent on the fish sample... and learned that my 1/8" parallels would not work without hitting vise jaws =)

Attachment 298222
Attachment 298224
Attachment 298226
Attachment 298228

[MetalShavings]

I'm finally caught up with my income-producing-work so tomorrow I have the day off. I'll be test-milling the "Action Wrench" project I posted earlier. I'll be using soft material to simulate my 1018 steel just to make sure it's going to work. If the general time of this HSM tool path hovers anywhere near the twelve-or-so minutes that were eluded to in one of the previous posts, I'll be able to finish them up before noon time.

I'm hoping for the best but bracing for the worst. If it goes off without a hitch I can set up my metal stock and machine it on Thanks Giving day. I'm not much of a football watcher so what better way to pass the time while I'm waiting for dinner to cook?

Wish me luck gentlemen. This will be my first venture into HSM. I'm hoping it will be a real time saver for me. I hope it works; I hope it works; I hope it works. Either way, I'll be back to let you know how it went.

MetalShavings

[MetalShavings]

Well, Hells-Bells!

The simulations were really encouraging. Cutting wood was a confidence builder and cutting air finally gave me the green-light to go ahead and try cutting my part out of metal.

It looked like it was really going to work. The first several passes had me grinning from ear to ear but when my end mill got about a quarter inch in it started bogging down big time. I couldn't figure out why because it was cutting the same WOC with each pass; or so I assumed. It was all happening to fast to really give it any lengthy thought so I opted to shut it down rather than risking any damage to my machine.

Who knows when I'll get another day off so I didn't waste any more time trying to tweak the input data on my SprutCam "Strategy" page to alter my HSM tool path. I went ahead and cut my part using conventional milling methods. Even though my parts came out fine using conventional milling I can't get over how fast my end mill was removing metal until it started bogging down. Just from standing there and watching the chips fly I could tell that this HSM method woud cut down my machining times tremendously.

There has to be something I missed or some set of numbers I entered incorrectly to not be able to get a finished part using HSM.


I thought I had it set to cut .015" at a time. My spindle speed was set correctly; according to the numbers given me. I'm going to have to go back and re-read all the posts on this thread to try to track down where I went wrong. I know this can work now. I just haven't figured out how to get it to work.

MetalShavings

[wtopace]

Sorry, I got busy with my day job and this thread fell below the radar.

Did you ever solve your issues?
Can you describe where it was bogging down? (a video might help tremendously)
Do you have a spindle load meter?

Generally in HSM, you should never bog any more in one part of the a cut than another, as your CAM package should keep the chipload the same everywhere (that's one of the key factors in HSM). Good to hear that you were at least somewhat successful!

[MetalShavings]

Sorry, I got busy with my day job and this thread fell below the radar.

Did you ever solve your issues?
Can you describe where it was bogging down? (a video might help tremendously)
Do you have a spindle load meter?

Generally in HSM, you should never bog any more in one part of the a cut than another, as your CAM package should keep the chipload the same everywhere (that's one of the key factors in HSM). Good to hear that you were at least somewhat successful!

I haven't yet resolved whatever issue caused the "Bogging-Down" effect. Perhaps even the .015 WOC was a bit much for this particular setup.

I was using HSM to cut the top half of my "Receiver-Wrench." I was using my four-flute .5" carbide coated end mill at one inch deep. .015" WOC and at the spindle speed listed in one of the initial replies. All seemed to be working wonderfully until about the sixth or seventh pass. That's when it started to bog down. I have no means to video these things: I don't have a "Spindle Load Meter" either.

At the time, I got the sense that if I'd used a shallower WOC it might have worked out better for me. The thing about HSM calculations is that to shallow of a cut is not good and to deep of a cut is not good. And if the properly calculated cut doesn't seem to work then you are left to decide wether to increase or decrease your feed rate, increase or decrease your spindle speed and possibly other alternatives; most of which I haven't a clue about.

If I had more free time I could play around with the numbers but as it is, these projects are done in between my regular income producing work schedule. This leaves me with precious little free time to do trial and error learning. Ideally, I'd like to get this figured out so that I enter the correct data into the data-fields in the "Strategies" page as well as any other pertinent input field pages in my CAM software.

MetalShavings

[SCzEngrgGroup]

I haven't yet resolved whatever issue caused the "Bogging-Down" effect. Perhaps even the .015 WOC was a bit much for this particular setup.

I was using HSM to cut the top half of my "Receiver-Wrench." I was using my four-flute .5" carbide coated end mill at one inch deep. .015" WOC and at the spindle speed listed in one of the initial replies. All seemed to be working wonderfully until about the sixth or seventh pass. That's when it started to bog down. I have no means to video these things: I don't have a "Spindle Load Meter" either.

At the time, I got the sense that if I'd used a shallower WOC it might have worked out better for me. The thing about HSM calculations is that to shallow of a cut is not good and to deep of a cut is not good. And if the properly calculated cut doesn't seem to work then you are left to decide wether to increase or decrease your feed rate, increase or decrease your spindle speed and possibly other alternatives; most of which I haven't a clue about.

If I had more free time I could play around with the numbers but as it is, these projects are done in between my regular income producing work schedule. This leaves me with precious little free time to do trial and error learning. Ideally, I'd like to get this figured out so that I enter the correct data into the data-fields in the "Strategies" page as well as any other pertinent input field pages in my CAM software.

MetalShavings

If you're bogging down with only 0.015" WOC, the last thing you want to do is decrease WOC. That is already very thin. And if you're bogging down, then your requesting more power than the spindle can provide. You pretty much never want to increase RPM, or feedrate, as either one will be abusing the tool through excessive SFPM. You either reduce depth, or width, generally whichever is greater. If your cut is already shallow, you don't want to make it shallower. If it's already narrow, you don't want to make it narrower. The whole idea behind HSM is to maintain a constant, high chipload, and to use as much of the length of the tool as possible. Increasing RPM reduces chipload, which is generally bad. Reducing feedrate reduces chipload, which is generally bad. Reducing depth has no effect on chipload, but does reduce power requirement, so is almost always the best thing to do.

Regards,
Ray L.