[CNC-Dude]

I am about to do a part which requires tapping. I watched the Sprutcam America tutorial and this seems straightforward enough. Except that I am getting the pesky red exclamation mark.

I am not certain if this feature was available on SC7 (I surely never found it), but according to SC9, the problem is being reported as "Gouge Of The Part". I have already drilled the hole to spec size. Where could the gouging come from?

If you have experienced this before, what was the solution? Thanks!

[mountaindew]

I would guess the hole size in your igs model is a little smaller then the tap outside or major diameter. sprut will see the tap tool as being to big for the hole and give you a gouge error.
When I design a part I draw the holes at clearance size. Then sprutcam is setup to drill to tap size and then setup a tap operation with no gouge errors because the tap cutting edge never touches the hole that is drawn at clearance size.
This is just one method of many. If you have the part drawn and don't want to change it then turn gouge detection off on that tap operation after you have verified that it is setup correctly. Also this forum also has some threads on setup guidelines for tension compression tap heads and the code it generates that are much more complete. Myself I like a delay at bottom of tap operation and a tool retraction point well above the part "0.5" to give the tool time to back out and reset. In my experience if you let sprut move to next hole at a small safe level that it many times it defaults to, it will leave part of the tap in the first hole.
Tap that
md

[MichaelHenry]

Check the SC9 G-Code and make sure that your feed and retract rates are correct.

Mike

[CNC-Dude]

Here is what I have tried. This used to work flawlessly on Sprutcam 7. Why, if SC9 is all but improvements, does such a simple task give has given me so many troubles? I guess it is a matter of getting that recipe jotted down. At least I know what DOESN'T work!

1. The IGS does not import the thread detail, as would be included within the model. Hence, when I double click on the threaded hole within SC9, the measuring tool tells me it is a 0.13" diameter hole.
2. Before threading, I have two Hole Machining operations. The first one is a spot drill and the second is a 9/64" drill (this is the drill I use for 8-32 TPI screws).
3. Here is the first problem, but oh well. The 9/64" drill diameter is actually 0.140625". Of course this would be a clash, as the hole is 0.13", so I trick the system and change the drill diameter to 0.13". The problem with the drill operation goes away.
4. Now comes the threading operation. I have defined the TAP as I have done many times and as specified in the video, but here is where all hell breaks loose! What I am seeing in the simulation is that the tap goes down to the bottom of the Z coordinates on the drill cycle (Z = -0.31108) and then the spindle turns on. EHHHH WHAAAAAAAAAAAAAAAAAAT???? My arrows are pointing up and I know the tap is coming from above the part's top. Why is the tap going to the bottom before the spindle turns on?

Also, I noticed that on this version of SC, the generated G Code does not have the dual feed rate as in SC7. If you recall, on SC7 the tap comes in faster than it comes out. You specify the feed rate and then something like a 10% multiplier is added to add/subtract from the nominal. Apparently on SC9 this is not required?

Needless to say I have tried a gazillion other things such as using different diameters for the drill and the tap operations and try to trick the SW, but I remain non victorious. As soon as I find the correct recipe I'll inform accordingly as this will most likely be one of those topics where many more will dwindle...

[mountaindew]

Cnc Dude
I don't draw threads, way to much work in my turn of the century cad software .
Sprut does everything with math and if the tap diameter is defined in the tool table even .0001 over the size of the hole that is drawn on the part it will give you a gouge error.
Is the tap defined in the tool table same as your drill "undersized" ? This will tell sprut your mathematically not touching any surface with the tap and you will not be gouging the part that way.
Your hole selection, top and bottom levels should be defined just like the other drill operations and the arrows and gfx should all look the same "no bottom up drilling".
The simulation I have no idea about motor turning or not, I don't look at this and its not a setting that can be turned on or off in the operation. Did you look at posted code to see when motor is on or off?

The feed rates and retract rates need to be set for best results along with a few others imho!

I will repost my notes on this subject. that have worked for countless holes . "I thought I posted this before but could not find it searching"
Look carefully at each parameter highlighted in yellow.


Sprutcam

Load sprutcam and default fixture model

Load part model and all other items required in the model for use mill operations and definitions

Parts and fixtures are translated into position and the machining tab is selected

Drill operations are first detailed and verified.

Select all holes and spot drill location




Define tap



Basic feeds and speeds

set rpm to 500 and cut speed

Feed calculation :

Imperial taps are (1/pitch x rpms)

Metric taps are (pitch x rpm / 25.4)



Then select and set plunge feed

and check % if work feed and set to 90





Select and set retract feed back to 100% if not default.



Strategy tab

select tapping with chip removal and Canned cycle

this enables dwell for top and bottom to be set as desired

Also STEP count must be set to 0 very important as this is not rigid and will break tool

safe distances or levels can also be set as desired "the 0.3 shown allows tc unit to recover and clutch back up





tool is configured

verify selected drilled holes and job assignments

simulate

Review g-code for the operation the clip below was pasted from the sprut 9 post dated 2.18.2015 and works fine
(Hole machining 8-32 Tap)
N310 T52 G43 H52 M6
(8-32 tap)
N320 G52 X0. Y0. Z0.
N330 S500 M3
N340 G0 X-0.875 Y0.
N350 Z0.4
N360 (Hole1)
N370 S500 M3
N380 G1 Z-0.65 F19.7
N390 M4
N400 G4 P0.3
N410 G1 Z0.3 F15.4
N420 M3
N430 G4 P0.4
N440 G0 X0.875 Z0.4

Note the feed rate changes also the pause at top and bottom are my additions , makes the operation slower overall but hey who wants to fiddle with broken taps.




Copied from my extensive note book I have hundreds of pages like this to help jog memory or a basis for a new setup .


Hope this helps!
md

[CNC-Dude]

MD, Thanks for this super valuable info! Man, you should have a blog or something on how to do all of these things. Those are quite the gold nuggets of information!

To report on my problem (and its inherent solution), I must confess this was yet another ridiculous problem caused by utter moronicity. And while I was cursing at the cosmos and punching all sorts of crap around the house, the only thing I should have been punching would have been my reflection on a mirror, as the utter moron is none other than... wait for it.... MEEEEEEEEEEEEEEEEE!!!!!

Check this one out. What happens when you design something to be cut on 0.325" stock aluminum but then only find 0.375" at your local metal store? ERRRRR!!!! You got it!

Of course Sprutcam was reporting gouging. Because I remembered to change the part width to 0.375" but not the hole depth. WHAMMO! Blind holes in the making.

It only took me about 24 hours to figure this one out and I must admit it was SC's transparency mode which gave it away.

As I am looking at the transparent mode (after long hours and a raspy throat due to all sorts of cursing), I stare at the holes and I see they are actually not going through. I am thinking "DARN YOU SPRUTCAM!!! WHAT WILL IT TAKE FOR YOU TO GIVE ME DARNED THROUGH HOLES????" I then realize it was me being the A-HOLE as I never gave SC a through hole to begin with. Went to the CAD and sure enough, WHAMMO! the holes were still 0.325" deep.

Oh well... You know how we say, No Pain No Gain! Well, it has been painful but the learning has been through the roof, so not all is lost. Now to finally get some darned chips flowing into the cosmos! Because I am well past late to deliver these motor mounts!

[mountaindew]

Noticed a new sprutcam video today on tc tapping "it was done a month ago" oops
And they show different settings to complete this operation.

Use long hand not canned cycle "this made little difference in code generated" in other words it does not generate canned cycle code with this post anyway but it does generate the correct feed rates when thread pitch is set to right value, detailed next.
Thread pitch needs to be set to threads per inch not pitch, in this case for a 8-32 it is set to 32 not 0.03125
Do not change plunge and work feed rates . they can be left at default 100%
They set pause at bottom only, the above example codes a pause at both top and bottom.

Good to see sprutcam is making some newer videos on how to use some of these settings. I didn't use long hand before because I didn't know about pitch setting change and it would generate incorrect feeds in the thousands.
This little bit of info cleared that problem up.
Hope they put out more videos
md

[CNC-Dude]

Yes, I had seen the video and that gave me an idea how to configure SC9. Except that I am still behind on tapping with SC9. On SC7, every single tap I did worked. With SC9 the tap broke right on the first hole. After that I just removed the tapping operation from the 4 parts I was building because I was running out of time and in this case I could live without the threads. Will need to spend a day just trying to figure this out. though. I don't do a lot of tapping but when I need it, it is handy like hell!

It was so easy on SC7. I wonder where did the programmers thought they were improving this feature because improved it is not! Not until I figure it out, at least.

[mountaindew]

I use a slow feed rate of 500. The new video was 3x that.
I use tap oil or I break taps.
I use 70% thread contact hole sizing with no problems, If I did have a problem I would oversize hole up to 50% thread contact size.
I see 0.00 changes in sprutcam. My only change is they explained the one parameter requires threads per inch not pitch as it is labeled.
This I would guess is a post processor thing and only applies to tormach not other machines. If it was other, then sprut would change the parameter label.
As for canned or long hand I used canned before because it generated the correct code "not a canned cycle as it states" and correct feed rates, again a post processor thing.

I did load and edit the 4 sizes of tap operations I have setup and then saved them back as user operations to use them in new part programs.
Also went into each one and carefully reviewed code generated by each one carefully. I found a few settings like safe heights and transition heights to be a little different and by setting all this consistently the code is much more optimized and less un needed z movements.

Hope this helps others zero in on methods that work for them.

[MichaelHenry]

With SC9 the tap broke right on the first hole.

Was the retract feed correct in G-code? The same thing happened to me on my first SC9 tapping op and it turned out the post had decided that the retract should be at twice the speed of the feed. I also use 500 rpm - that seems to be fast enough so the motor/tap is not torque-limited and slow enough that there's a chance of stopping the code if something doesn't look right.

Mike