[ChrisPhoenix]

This part was imported from Autodesk Inventor using the import plug-in. So no IGES problems this time. The other half of the mold worked great in SprutCam - just about the easiest file I've prepared yet. But this one...

I have a tool that's the same size, or slightly narrower, than the slot I'm trying to cut (I've tried it both ways). It refuses to cut to the end of the slot, or go down the hole. If I set the tool much narrower (0.06 rather than 3/32), then it does. It seems to be stopping at a point when the height of the cut changes.

But this is not a very complex part! Why is it acting crazy? I've tried lots of operations, and nothing works, and some of them do weird stuff like doing one or two waterline passes around the entire circumference of the part (at least if I try to include both symmetrical flats).

Thanks,
Chris

[Gerry Sweetland]

This part was imported from Autodesk Inventor using the import plug-in. So no IGES problems this time. The other half of the mold worked great in SprutCam - just about the easiest file I've prepared yet. But this one...

I have a tool that's the same size, or slightly narrower, than the slot I'm trying to cut (I've tried it both ways). It refuses to cut to the end of the slot, or go down the hole. If I set the tool much narrower (0.06 rather than 3/32), then it does. It seems to be stopping at a point when the height of the cut changes.

But this is not a very complex part! Why is it acting crazy? I've tried lots of operations, and nothing works, and some of them do weird stuff like doing one or two waterline passes around the entire circumference of the part (at least if I try to include both symmetrical flats).

Thanks,
Chris

Hi Chris,
I measured between the walls on both of those slots in SC and got .0938" in the one on the left and .0937" in the other. You have a tool that is entered as Ø0.09374". I changed it to 0.093" and it ran the whole length of the slot. In the attached file I added the other slot to the operation and it ran that as well. I don't know know why the slot you were trying to simulate (the left one) would not machine full length when your tool Ø was under by 0.00006"? Changing the tool Ø to 0.093" seemed to fix it though? Maybe a tolerance thing in SC?

I think there are still some issues with your model though. I question why there are so many different faces on the top surface? I have never worked with Inventor, well I did play with a demo a couple of years ago, maybe that is what is supposed to do? I have been using SolidWorks for about 12 years and before that mostly CadKey and some 2D AutoCad mixed in. In an exported SW model to .iges there would not be all those face segments in the file. I could try to reproduce your model or something similar in SW and show you what the imported .iges file would look like in SC if want me to. I don't know how much you are invested in AutoCad Inventor but if you have the opportunity take a look at SolidWorks.
HTH
Gerry

I forgot to mention that in the attached file I did a couple of other minor additions, such as changed Lead in-Lead out to a safe height to .1 etc.

[ChrisPhoenix]

Argh - I tried setting the tool to 0.900 and it did not machine to the end! And the two slots were created with "mirror" in Inventor, so they should be exactly the same width as each other (and the tool).

At least some of the facets on the top are because I "sliced" the part a few times in Inventor. I wouldn't expect them to cause a problem, in a sane program.

Using IGES does cause problems - the file comes in with lots of zero-width "railings" around level-changes that cause SprutCam to act extremely crazy - cutting through the part and not noticing, removing entire features, etc.

I'm using the Inventor/SprutCam combination because they're available free at TechShop.

Inventor does cause problems sometimes - I haven't been able to make 3D patches work with the mold tool, for example. But SprutCam is far worse - it crashes several times a day, it does crazy things for no apparent reason (like cutting through parts, or setting spindle speed to 200 - good way to break a tool), and the user interface design is very difficult to use. Out of the two, if I were going to pick a tool to recommend AGAINST, it would absolutely be SprutCam.

I'll try your file and see whether it generates correct toolpaths on the TechShop installation. Thanks!

Chris

[ChrisPhoenix]

Thinking further - is there any setting in SprutCam that could affect the precision with which it imports files from Inventor? I'm remembering that when I tried to measure the part, points along the top edge had a Y slightly greater than 0. I thought it was SprutCam not snapping to the point (although I had "smart snap" turned on), but now I'm wondering if the part simply imported too imprecisely.

And another question - have you found any way to change the precision in the color display that shows blue for rest material and red for gouges? (Sorry, I can't find the name in the manual, and don't have the software in front of me). Even when I change the numbers in the little floating window, it doesn't seem to change the tolerances-to-colors mapping that's displayed.

Thanks,
Chris

[Wirecutter]

This part was imported from Autodesk Inventor using the import plug-in. So no IGES problems this time. The other half of the mold worked great in SprutCam - just about the easiest file I've prepared yet. But this one...

I have a tool that's the same size, or slightly narrower, than the slot I'm trying to cut (I've tried it both ways). It refuses to cut to the end of the slot, or go down the hole. If I set the tool much narrower (0.06 rather than 3/32), then it does. It seems to be stopping at a point when the height of the cut changes.

But this is not a very complex part! Why is it acting crazy? I've tried lots of operations, and nothing works, and some of them do weird stuff like doing one or two waterline passes around the entire circumference of the part (at least if I try to include both symmetrical flats).

Thanks,
Chris

Disclaimer: I am quite a rookie with SprutCam, and I bow in deference to Gerry. I don't post much yet because I haven't developed very many 'non-stupid' questions.

But going to the original question: So far, the operations that I've been able to get the most out of are the waterline ops. But by default, they'll try to machine everything, it seems. (Yeah, I need to search the forum and re-read how to assign jobs (features) to the waterline ops.) Of course, I limit the depth of the waterline ops in the parameters tab because the part is held in a vise. I picked up a somewhat slimy hack from one of the tutorial videos. If I want SC to leave an area alone, I go to the "2D Geometry" tab and draw a closed shape around it. Either polygon-by-points, circle, whatever. Then go back to the "Machining" tab. Select fixtures. Extrude the 2d shape to the min and max height that I want. I can do this for individual operations, but keep an eye on subsequent ops, because the "fixtures" created this way will, by default, get inherited by later ops.

I had to do this in one of my recent projects. I did a roughing waterline with a roughing mill, then a few drilling and other operations. The last operation was finish waterline with a ball-end mill. It runs around and over the various features until it's nearly done. Then, for some infuriating reason, SC would have the ball-end mill "kiss" a couple of shallow drilled holes. (.250" ball mill plunges about .080" into a couple of .156" holes, pretty much wrecking them.) Gaaaah! I checked the parameters of the operation several times, re-ran over and over, but no luck. So, I wound up creating a couple of "cylindrical fixtures" inside the holes using the method above. This finally got the finishing waterline operation to leave the holes alone.

I now use this technique probably more than I should, but I'll keep doing it until I know better. I need to read this forum more.

-Mark

[ChrisPhoenix]

Mark, yup, that sounds like the SprutCam I know and loathe. I've been using SprutCam for months, and it does not get better.

When I referred to "IGES weirdness" that was in reference to another thread of mine. Either Autodesk Inventor or SprutCam has a bug with IGES files, and my files had extra zero-width features that apparently confused SprutCam and made it machine right through features. It would go around the edge of a boss carefully, doing proper waterline steps, then do a sort-of-flat-land-finishing operation that removed the boss completely. Setting a restrict zone did not help. So, try importing your part differently, and be on the lookout for a different set of weirdness when you do. I still haven't found a way to import from Inventor to SprutCam that works every time. (The plugin doesn't preserve exact dimensions.)

Thanks for the tip about creating fixtures to make SprutCam leave a region alone. Restrict zone just does not seem to work right (at least sometimes).

When SprutCam is working right, simply selecting facets of the part and clicking "Add Faces" will make it do only those faces rather than the whole part. I've also found that creating a workpiece that's the same size as the part will sometimes avoid the annoying "run around the outside all the way down" behavior.

Chris

[ChrisPhoenix]

I found one of my problems. SprutCam, for some reason, rounds to 0.001" precision when selecting a tool from the library. So if the tool is 3/32, and I put 0.09375 as the diameter, it shows up that way in the library... and then when I select the tool, it sets the diameter to 0.094. If the slot is 0.09375, it won't machine it.

But that's not the whole problem. It doesn't explain why it machined only part of a parallel slot. And doesn't explain why a 0.08 tool won't do flat land finishing in a 0.09375 hole, but a 0.07 tool will.

If you don't see me on this form again, it's because I've managed to make InventorCam work. I HOPE!!!

[adamvs]

But going to the original question: So far, the operations that I've been able to get the most out of are the waterline ops. But by default, they'll try to machine everything, it seems. (Yeah, I need to search the forum and re-read how to assign jobs (features) to the waterline ops.) Of course, I limit the depth of the waterline ops in the parameters tab because the part is held in a vise. I picked up a somewhat slimy hack from one of the tutorial videos. If I want SC to leave an area alone, I go to the "2D Geometry" tab and draw a closed shape around it. Either polygon-by-points, circle, whatever. Then go back to the "Machining" tab. Select fixtures. Extrude the 2d shape to the min and max height that I want. I can do this for individual operations, but keep an eye on subsequent ops, because the "fixtures" created this way will, by default, get inherited by later ops.

I had to do this in one of my recent projects. I did a roughing waterline with a roughing mill, then a few drilling and other operations. The last operation was finish waterline with a ball-end mill. It runs around and over the various features until it's nearly done. Then, for some infuriating reason, SC would have the ball-end mill "kiss" a couple of shallow drilled holes. (.250" ball mill plunges about .080" into a couple of .156" holes, pretty much wrecking them.) Gaaaah! I checked the parameters of the operation several times, re-ran over and over, but no luck. So, I wound up creating a couple of "cylindrical fixtures" inside the holes using the method above. This finally got the finishing waterline operation to leave the holes alone.

I now use this technique probably more than I should, but I'll keep doing it until I know better. I need to read this forum more.

-Mark

I've had pretty good luck using the same technique to define a job zone, without extruding them. I click on the defined region and make sure the tool is confined to that area. Perhaps in a situation like you described you could use the hole boundary as a restricted zone. I also using 2D geometry to create a tool path for a 2D contour op for roughing out big areas of material with face mill and follow with waterline roughing, using a smaller diameter mill for the details - it works pretty well!

[dbrija]

Argh - I tried setting the tool to 0.900 and it did not machine to the end! And the two slots were created with "mirror" in Inventor, so they should be exactly the same width as each other (and the tool).

At least some of the facets on the top are because I "sliced" the part a few times in Inventor. I wouldn't expect them to cause a problem, in a sane program.

Using IGES does cause problems - the file comes in with lots of zero-width "railings" around level-changes that cause SprutCam to act extremely crazy - cutting through the part and not noticing, removing entire features, etc.

I'm using the Inventor/SprutCam combination because they're available free at TechShop.

Inventor does cause problems sometimes - I haven't been able to make 3D patches work with the mold tool, for example. But SprutCam is far worse - it crashes several times a day, it does crazy things for no apparent reason (like cutting through parts, or setting spindle speed to 200 - good way to break a tool), and the user interface design is very difficult to use. Out of the two, if I were going to pick a tool to recommend AGAINST, it would absolutely be SprutCam.

I'll try your file and see whether it generates correct toolpaths on the TechShop installation. Thanks!

Chris

The spindle speed at 200RPM happens via the way you create a tool. The fix is to pick an appropriate operation (i.e. create a pocketing operation), open that operation, and in "Tool", define the tool properties (diameter, length, etc... but do not "Add" or "Replace" yet), then go to "Feeds and Speeds" in the operation, and set your spindle speed, feedrate, coolant on or off, go back to the tool screen, and "Add" or "Replace". Otherwise, you get the 200RPM default.

Note also that the tool info is just a .csv and you can edit it in Excel to fix these things.