Stock on facing

[dfox1787]

This is confusing as magicniner asked "is the top of your part zero" and you said "yes" and then said left bottom corner is set to zero!!

The normal way to start is to use the top of the part as Zero and any movement below that becomes -ve

Well it's the top of the stock but in the corner. So it's still the top it's just I prefer my zero position in the corner.

Also the facing operating is removing the correct amount off the stock it looks like the pocket operation after isn't taking that into account.

Sent from my SM-N910F using Tapatalk

[magicniner]

Well it's the top of the stock but in the corner. So it's still the top it's just I prefer my zero position in the corner.

Your Stock is not your Part, that kind of confusion will result in unexpected depths of cut when you incorrectly interpret the terminology in your CAM package :D

[dfox1787]

Your Stock is not your Part, that kind of confusion will result in unexpected depths of cut when you incorrectly interpret the terminology in your CAM package :D

i know its not but ot shoudl take into account the stock is thicker than the part and the take .45mm off the pocket if the stock has been faced.

the first operating is a face to remove .45 and the next is a hole pocket and the operating after is to pocket 2mm not 2.45mm. On the simulation the z moves down to 2.45mm

http://a360.co/2mUUlN4

[magicniner]

You are mixing things up and trying to make the CAM work the way you think it should.
It's obvious that you are taking .45 off your stock but referencing your pocket depth as it would be from Top of Stock but your CAM is taking it from the actual Top of Part.
Setting Top of Stock as Top of Part is the source of your issues, you'll have to work out how to juggle the numbers in CAM to deal with that, a spreadsheet would help in keeping track of the differences required ;-)

[dfox1787]

You are mixing things up and trying to make the CAM work the way you think it should.
It's obvious that you are taking .45 off your stock but referencing your pocket depth as it would be from Top of Stock but your CAM is taking it from Top of Part.
Setting Top of Stock as Top of Part is the source of your issues, you'll have to work out how to juggle the numbers in CAM to deal with that, a spreadsheet would help in keeping track of the differences required ;-)

thats correct. i would it expect it to know i already removed .45mm from the facing operation. I have to add a offset of -.45 for the tool path to start at the correct depth but it still pockets -2.45 which is going to make the the pocket deeper than it should be. At the moment the only way i can see is to leave it cutting nothing but it adds machining time. . To me it should know have took that into consideration.

Unless there is a setting im missing.

but if the fusion doesn't calculate it that it just adds more time for me creating paths. thank you for your response as always :)

[magicniner]

Your time creating paths would be normal if you follow industry conventions.

Top of Part should be the top of your part, your stock should be defined correctly within the software and your CAM can then see what is required for a facing cut on the top of the part, without you defining the depth of material to be removed, because it knows the depth of stock above the part. You just tell it the depth of cut you want to use with your cutter and the CAM will work out if it needs one or more passes.

[dfox1787]

Your time creating paths would be normal if you follow industry conventions.

Top of Part should be the top of your part, your stock should be defined correctly within the software and your CAM can then see what is required for a facing cut on the top of the part, without you defining the depth of material to be removed, because it knows the depth of stock above the part. You just tell it the depth of cut you want to use with your cutter and the CAM will work out if it needs one or more passes.

I should be able to tell the tool path to start the at 6mm and pocket -2mm. At the moment no matter what i change it always pockets -2.45mm.

here is the part if you want to take a look http://a360.co/2mUUlN4

[Neale]

thats correct. i would it expect it to know i already removed .45mm from the facing operation. I have to add a offset of -.45 for the tool path to start at the correct depth but it still pockets -2.45 which is going to make the the pocket deeper than it should be. At the moment the only way i can see is to leave it cutting nothing but it adds machining time. . To me it should know have took that into consideration.

Unless there is a setting im missing.

First of all, You haven't given us quite as much information as I would like - a screenshot showing the CAM model with the various heights shown would help, along with a copy of the setup/operations list on the LH side of the screen. So what I say here is guessing at what these might show but this is based on my own use of F360 (which I use a lot for design and CAM).

Based on what I think you are doing, two quick answers. First of all, F360 is doing exactly what you told it to. No more and no less. Secondly, it will cut your pocket to exactly the correct depth as you have it; the simulation shows the pocket depth being 2.45mm deep. That's not an error - in the operation tab, you told it to work with top height equal to stock top - and the pocket is 2.45mm deep from stock top. Best way to fix this is just to change "top height" to reference model top, not stock top. That should work OK.

What I am not sure about because I can't see exactly how you have set up your operations is whether it will start cutting from stock top (so cutting air for 0.45mm) or from model top. I would create one setup and then under that create two (or more - not sure what else you are doing) operations. The first is to face the stock and second is to cut the pocket. I've just thrown a quick F360 model together and tried the CAM operations. I used facing and pocket under 2D (you can use 3D pocket clearing but this just complicates things when you are really cutting a 2.5D feature) and running the simulation it seems to do exactly what you want - the pocket cut starts at the top of the model, not the stock.

I would disagree with Nick - you might only be doing 2.5D operations (that is, essentially 2D but with a single defined depth of cut) but I don't see any issue in putting the 3D model together. It takes a minute or two to do, gives you all the F360 advantages (although this depends on what you are comparing it with) such as being able to go back to the drawing and change a dimension and have everything dependent on that automatically change or be marked to be recalculated. Nick is much more experienced than I am, as I always assume that I am going to make mistakes and F360 gives the best chance to go back and make changes without redrawing. In addition, of course, this might be just one component of a more complex 3D design in which case designing in F360 and then applying CAM to individual components for CNC manufacture is a sensible way to go. Practising on individual components makes this a good training exercise anyway.

My model took only a few minutes to generate; it can be edited trivially, can be rotated on screen for visualisation, etc. I, personally, like working with a relatively simple-to-use 3D tool like F360, but there's plenty of scope for other views and a lot depends on what you are used to. I've been at a model engineering exhibition today, talking to quite a few professional engineers from various backgrounds from aerospace to watch-making, and everyone has their own favourites. Largely determined by what their employer has bought and standardised on, but not many people buy their own Catia or Solidworks!

[dfox1787]

First of all, You haven't given us quite as much information as I would like - a screenshot showing the CAM model with the various heights shown would help, along with a copy of the setup/operations list on the LH side of the screen. So what I say here is guessing at what these might show but this is based on my own use of F360 (which I use a lot for design and CAM).

Based on what I think you are doing, two quick answers. First of all, F360 is doing exactly what you told it to. No more and no less. Secondly, it will cut your pocket to exactly the correct depth as you have it; the simulation shows the pocket depth being 2.45mm deep. That's not an error - in the operation tab, you told it to work with top height equal to stock top - and the pocket is 2.45mm deep from stock top. Best way to fix this is just to change "top height" to reference model top, not stock top. That should work OK.

What I am not sure about because I can't see exactly how you have set up your operations is whether it will start cutting from stock top (so cutting air for 0.45mm) or from model top. I would create one setup and then under that create two (or more - not sure what else you are doing) operations. The first is to face the stock and second is to cut the pocket. I've just thrown a quick F360 model together and tried the CAM operations. I used facing and pocket under 2D (you can use 3D pocket clearing but this just complicates things when you are really cutting a 2.5D feature) and running the simulation it seems to do exactly what you want - the pocket cut starts at the top of the model, not the stock.

I would disagree with Nick - you might only be doing 2.5D operations (that is, essentially 2D but with a single defined depth of cut) but I don't see any issue in putting the 3D model together. It takes a minute or two to do, gives you all the F360 advantages (although this depends on what you are comparing it with) such as being able to go back to the drawing and change a dimension and have everything dependent on that automatically change or be marked to be recalculated. Nick is much more experienced than I am, as I always assume that I am going to make mistakes and F360 gives the best chance to go back and make changes without redrawing. In addition, of course, this might be just one component of a more complex 3D design in which case designing in F360 and then applying CAM to individual components for CNC manufacture is a sensible way to go. Practising on individual components makes this a good training exercise anyway.

My model took only a few minutes to generate; it can be edited trivially, can be rotated on screen for visualisation, etc. I, personally, like working with a relatively simple-to-use 3D tool like F360, but there's plenty of scope for other views and a lot depends on what you are used to. I've been at a model engineering exhibition today, talking to quite a few professional engineers from various backgrounds from aerospace to watch-making, and everyone has their own favourites. Largely determined by what their employer has bought and standardised on, but not many people buy their own Catia or Solidworks!

Hi Neale

Thank you for your reply.

Sorry i am still new to fusion and current use aspire which i know functions totally different.

You are correct in staying the the pocket operation does hover over the part if it has already been faced. I have tried to set the tool path to the top of the model which does work on the simulation. The thing that is confusing for me is that on the simulation the pocket z height still cuts to -2.45mm. (maybe this is correct)

I did look at how to do the simple outlines function as nick asked but couldn't see how to set the cut depths but again that is probably me still not sure how the software works. With the little time i have. I spent watching online videos showing how to use fusion but i haven't yet found one where the stock is set to a fixed size because the material i will be using has these fixed dimensions.

One thing i did notice is if i set the facing operation the last thing i did and selected the one face that would be left after the previous tool paths then there are no issues. Perhaps this is the way the software is designed and the facing is meant to be the last thing you do?. Again still learning how to use the software.

heres a copy of my fusion file if you want to have a look.

http://a360.co/2mUUlN4

[magicniner]

Sadly not harsh, repeated explanations ignored culminating in-

thats correct. i would it expect it to know i already removed .45mm from the facing operation. I have to add a offset of -.45 for the tool path to start at the correct depth but it still pockets -2.45 which is going to make the the pocket deeper than it should be. At the moment the only way i can see is to leave it cutting nothing but it adds machining time. . To me it should know have took that into consideration.

Unless there is a setting im missing.

but if the fusion doesn't calculate it that it just adds more time for me creating paths. thank you for your response as always :)

Fusion 360 should know he's taken .45 off the stock (the top of which he's set as zero) and compensate for him but unfortunately Fusion 360 has the same problem as me, it's Crystal Ball is in for repair! :D