Stock on facing

[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

[magicniner]

It's a 2.5D part and you've modelled it in 3D and are using the 3D model in CAM?
There's your extra work! :D

To generate the paths you need in CAM for true 3D parts you will at some point need additional geometry as well as your 3D part, this geometry can be as simple as a perimeter to limit a cutting path to exactly the area you want or as complex as extending a compound curved surface beyond the edge of your model to allow a smooth finishing tool path to transition off and back onto the part for an axis feed rather than stopping exactly at the edge and creating machining artifacts.

Similarly for 2.5D parts you rarely need much if any part modelling and can control your tool paths with very simple, easily constructed geometry, this is why there are still people out there who think CAD/CAM for a single simple part is slower than manual machining, most often it's not ;-)

Just draw all your geometry at Z zero and generate paths to your required depths for
1. Facing cut
2. Rectangular Pocket
3. Through Hole

The geometry for your facing cut will be larger than the part perimeter by just more than your cutter diameter
The geometry for your rectangular pocket will be larger in two directions by just more than 1/2 your cutter diameter
The geometry for your round pocket will be unchanged.

In my CAD/CAM that takes me around 8 minutes to draw and tool-path

Modelling simple 2.5D parts in 3D is not required unless -
You need the part for a complex 3D assembly in CAD,
You can't visualise the part without pretty pictures,
The customer wants pretty pictures,

[dfox1787]

It's a 2.5D part and you've modelled it in 3D and are using the 3D model in CAM?
There's your extra work! :D

To generate the paths you need in CAM for true 3D parts you will at some point need additional geometry as well as your 3D part, this geometry can be as simple as a perimeter to limit a cutting path to exactly the area you want or as complex as extending a compound curved surface beyond the edge of your model to allow a smooth finishing tool path to transition off and back onto the part for an axis feed rather than stopping exactly at the edge and creating machining artifacts.

Similarly for 2.5D parts you rarely need much if any part modelling and can control your tool paths with very simple, easily constructed geometry, this is why there are still people out there who think CAD/CAM for a single simple part is slower than manual machining, most often it's not ;-)

Just draw all your geometry at Z zero and generate paths to your required depths for
1. Facing cut
2. Rectangular Pocket
3. Through Hole

The geometry for your facing cut will be larger than the part perimeter by just more than your cutter diameter
The geometry for your rectangular pocket will be larger in two directions by just more than 1/2 your cutter diameter
The geometry for your round pocket will be unchanged.

In my CAD/CAM that takes me around 8 minutes to draw and tool-path

Modelling simple 2.5D parts in 3D is not required unless -
You need the part for a complex 3D assembly in CAD,
You can't visualise the part without pretty pictures,
The customer wants pretty pictures,

are you saying to make a 2d model and create tool paths from that? i cant see how it can know the depths i need to face and pocket from a 2d model. I thought i could make my own model within the model and the machine it out in cam.

[magicniner]

are you saying to make a 2d model and create tool paths from that? i cant see how it can know the depths i need to face and pocket from a 2d model. I thought i could make my own model within the model and the machine it out in cam.

No, you don't need any models at all!
I'm saying that all you need is two rectangles and one circle drawn at Z = zero and use them to control tool paths.

i cant see how it can know the depths i need to face and pocket from a 2d model.

Autocad state that it is possible to 2d pocket from chained contours, that's lines to you and me, not solids, not 2d faces but lines.
One of the options for Bottom Height is Stock top: incremental offset from the Stock Top. so you set your depth as an offset from Z Zero, which is also top of stock, making things easy for yourself rather than trying to make it complicated then trying to make that work!

Here's a link to a relevant page on TFM, give it a read -
http://help.autodesk.com/view/fusion...D-B28D938D146E

[dfox1787]

are you saying to make a 2d model and create tool paths from that? i cant see how it can know the depths i need to face and pocket from a 2d model. I thought i could make my own model within the model and the machine it out in cam.

sorry i dont understand why it cant be done the way im doing it and why its complicated. i've seen plenty of videos of people creating a model on fusion 360 and then using the cam to machine it. (https://www.youtube.com/watch?v=o-GBpUZ3piY&t=134s)

I know i can do the same operating in aspire where i can surface the stock first and then set the start cut depth. so if i remove .45mm from the stock i can start the cut -45mm but to me fusion seems to make the same operation more complex or not very easy to understand.

aspire is simple:



Fusion does appear to have better tooling operations so i am keen to understand it more and use it for future projects. i am still new to it but something as simple as removing some materiel and then start the cut from the depth i want seems impossible at the moment.

[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