PDA

View Full Version : Fill in my knowledge gap :)



Davek0974
01-06-2016, 11:55 AM
My CNC experience is related to plasma cutting and more recently my mini-mill which so far has only been used to cut profiles from flat sheet and put holes etc in them as needed. I use Aspire or SheetCam for the CAM.

I am now converting my Bridgeport to CNC to expand my possibilities, all 3 axes will be controlled.

I need to make some parts for the Z axis drive and these can be done on my mini-mill which is handy as the Bridgeport is in 1000 pieces at present ;)

However, with my limited 2D knowledge so far, it was not until started modifying the drawings which were kindly sent to me by a previous converter that i realised how little I know about making the file for a 3D part :ambivalence:

18537
The picture shows various views of it, it has features on front and back, holes, a large slot etc.

I know pocketing, contouring etc but what is the missing link here?

My guess was to machine all the front details, holes and the outside first from a larger lump of plate, this would give me a part with the edges to size and one side finished.

Then, flip over, pick up my X & Y datum from whatever corner I use, and machine the back face - this is where I hit the knowledge gap - do I remove the outline (it's finished) and convert the features needed (a T-shaped slot) into full outlines on their own or something else??

I have never seen any other CAD source and my 2D stuff seems very simple compared so???

lucan07
01-06-2016, 12:16 PM
I am as new as you at this but in fusion I would create front as required and then copy that whole object flip 180 deg and add back detail to second copy.

Then use blocks fixed on bed to ensure accurate placement when flipping before starting to machine the reverse after contour cut before removing piece adding blocks for placement.

2 single 2d operations on one part if that makes sense.

Davek0974
01-06-2016, 12:25 PM
Yes, but the paths for the reverse - do these have to be just the T-shape pocket required

i.e. the front would be the whole object and the back would look just like a large T shape with no outline at all?

lucan07
01-06-2016, 12:45 PM
Yes only cut the slot and contour once then flip to machine only what could not be machined from front, so back would just be a T shaped pocket to required depth. I would start from same corner point on second setup but on other side of material obviously. Although placement may be easier to cut slot and T Pocket and holes first and then flip to cut remaining front using holes and pockets to fix back down.

Davek0974
01-06-2016, 12:59 PM
The slot is pretty wide so i would position the material to place the eventual slot over a run of bed holes, machine the slot plus the two small ovals, then fit clamps into the slot and finish the rest of the front.

As you said, then place blocks on bed touching the finished edge, flip over, clamp around the edge and machine the pocket T.

Seems to make sense now, will finish the drawings and do a simulation or two :)

Thanks

Davek0974
07-06-2016, 09:23 PM
A little more gap to fill...

How do you program an edge chamfer or break an edge in CNC??

I have Aspire but no idea on this one?

I would guess at using a 45deg tool but is there a method to offset the correct amount and set the depth?

JAZZCNC
07-06-2016, 09:37 PM
A little more gap to fill...

How do you program an edge chamfer or break an edge in CNC??

I have Aspire but no idea on this one?

I would guess at using a 45deg tool but is there a method to offset the correct amount and set the depth?

The Cam software will most likely have Chamfer toolpath which will give parameters such as chamfer length then take the tool size/angle and do the offset for you.

If not then it's bit of math for depth/length which I've no clue about and setting an offset. To save my brain I just use Cad to show me how deep/offset etc.

needleworks
07-06-2016, 09:39 PM
A little more gap to fill...

How do you program an edge chamfer or break an edge in CNC??

I have Aspire but no idea on this one?

I would guess at using a 45deg tool but is there a method to offset the correct amount and set the depth?
I am no expert by any stretch of the imagination, and I also struggled with this one ! What I ended up doing was just a case of simple maths, taking your 45deg cutter, You could assume that 0, 0, 0, puts the tip of the cutter right on the edge of your part, I then just told mach3 that I was using a 4mm cutter (doesn`t matter what size you insert here as long as it corresponds with your depth of cut) and used a cutting depth of 2.5mm. This in turn would put a .5 chamfer (in my case just a regular countersink) right round the edge of your part. If you required a larger chamfer, then simply lower the cutter to a depth of 3mm. Hope you can understand what I`m trying to say here:thumsup:

lucan07
07-06-2016, 09:39 PM
Only do this in Fusion but just use a 2d chamfer and select a chamfer mill to suit.

Davek0974
07-06-2016, 10:02 PM
Thanks all, seems this function is a downloadable option for Aspire but as I'm running an older version of the software it's not available for me, oh well, looks like i'll be needing that math knowledge I didn't learn at school again....


:)

Yes the explanations make sense and I have an idea now of what to try.

routercnc
07-06-2016, 11:36 PM
Hi Dave,

Just knocked this together to help work it out.

You can use one of the 3 look up tables depending on if the chamfer tool is 90, 60, or 45 deg.

Then assuming you use a notional tool diameter of 4mm as suggested above by needleworks in the CAM tool definition, then you just need to look up the required chamfer distance you require (C) and read off the depth of cut required (P) and enter this value into the CAM software.

I've not tried this out but I think it is OK. Please check on a scrap piece first (!).

Any errors spotted by anyone let me know . . .

18590

lucan07
07-06-2016, 11:39 PM
Maybe install fusion and only use it for your first hundred thou, cut the bevels in april before your turnover too high, or just set up all your regular jobs requiring bevels on 30day trial.

Davek0974
08-06-2016, 08:57 AM
Maybe install fusion and only use it for your first hundred thou, cut the bevels in april before your turnover too high, or just set up all your regular jobs requiring bevels on 30day trial.

I tried Fusion360, couldn't figure it out at all, Aspire I can grasp, SheetCam is easy :)

needleworks
08-06-2016, 09:50 PM
Hi Dave,

Just knocked this together to help work it out.

You can use one of the 3 look up tables depending on if the chamfer tool is 90, 60, or 45 deg.

Then assuming you use a notional tool diameter of 4mm as suggested above by needleworks in the CAM tool definition, then you just need to look up the required chamfer distance you require (C) and read off the depth of cut required (P) and enter this value into the CAM software.

I've not tried this out but I think it is OK. Please check on a scrap piece first (!).

Any errors spotted by anyone let me know . . .

18590
Yes, that explains it a lot clearer mate :beer: I should also have said that I use cambam for my toolpaths (not mach3 as I said in my previous post) like many, I just can`t get to grips with fusion 360 cause it always seems to mess up somewhere.

Davek0974
05-07-2016, 09:23 PM
Looking for suggestions on how to do the CAM for a part i make batches of manually at present, it's a round shaft with a square peg on the end. I have the vise mounted usually in one place for long periods so a G5x offset seems good, I can ref off the fixed jaw front and end.

It's not shown in my sketch but the radius of the tool is used to create a radius at the point where the square peg meets the body - just run the tool in from the end.

The part is held in a square 5C collet block at a fixed depth, the vice is fitted with an end-stop so pretty much all settings are repeatable and fixed.

I am looking to machine two sides and the end, rotate the block 90deg and re-run.

18860

Just looking for ideas :)

m_c
06-07-2016, 12:17 AM
In all honesty, I wouldn't bother with CAM.

I'd probably hand code using work offsets. Use a reference point (i.e. touch of end of material, then touch of the side) to zero the work piece coordinates, then hand code based of that.

At most I'd use the Mach wizards to generate the code for each side, if multiple passes on each side is needed.

Davek0974
07-07-2016, 04:26 PM
Hmm, thats a leap forward, not hand-coded anything yet ;)

Once the refs are made - end for X and centre of rod for Y, i can see saving them as offsets - they will not change unless the vise is moved which does not happen too often. So i just need to figure the path out i guess.

The manual ones i cut in one pass, its a little heavy on the tool but works ok, with automation i would likely use two passes as the steel is harder than plain mild.

ptjw7uk
08-07-2016, 12:34 AM
Why not do them vertically then you wouldn't have to move them.
If you want the radius use a round nose cutter.

Peter

Davek0974
08-07-2016, 08:13 AM
Thats an interesting thought, thanks.

Cutting forces would be harder to resist but not impossible, I have a 5C collet holder with vertical/horizontal bolt-down base, could use that if it grips well enough.

Will need to test this when i get her running :)

Davek0974
10-07-2016, 08:30 PM
Ok, next thing :)

How can i pick up an edge without a working edge-finder?

I tried today using my normal edge-finder but that likes to run at about 800rpm and the mini-mill does not go below 1000. Also it does not have a spindle-toggle button (yet) so i tried an MDI of M03-s1000 which works of course but then you cant jog the axis as it on the MDI line, moving off the MDI seems to upset the speed control which then starts wandering all over the place.

Maybe i'm missing something here?

For this job a simple pointed probe worked but the next part I have needs machining both sides accurately so i need a way to pick up the reverse spot-on.

Ger21
10-07-2016, 08:56 PM
Put an precision rod in the spindle and use the 2010 Probing wizard?

Davek0974
10-07-2016, 09:02 PM
but that needs an insulated workpiece or spindle to function no?

m_c
10-07-2016, 09:39 PM
How accurate does it have to be?

I've been known to just slowly jog in with an endmill going at slow(ish) speed until it just touches the material.

Davek0974
10-07-2016, 09:40 PM
Well, pretty accurate i guess - features on both sides have to match up ;)

m_c
10-07-2016, 10:49 PM
It should be just as good as edge finder, but it'll depend on how good your eyesight is ;-)

Davek0974
20-07-2016, 10:58 AM
Ok, the tool length offset table ;)

I'm going to try R8 ER collet chucks as a repeatable method of tool holding, have asked many people and resounding reply was yes it should be plenty accurate enough for this style of machine.

1 - With the tool offsets, can I measure them using the Z axis probing and touch-plate setup?

2 - I guess i need a "default tool zero" or some such to enable a reference length to be kept and then measure all tool against that one?

3 - If i was using the tapping head, i would need to lower the knee about 5", ref the surface again, tap the threads then return the knee to the higher position. Fit the next tool, set the tool number in Mach3, ref the surface and good to go again??

Am i on the right tracks here?

Davek0974
05-08-2016, 12:46 PM
Well, i now have a Haimer 3d-Taster for edge referencing, nice little tool, if i ever get the mill project finished it will come in handy ;)

I also have a bundle of ER32/R8 collet chucks for tool-holding.

And I have just about sussed out tool length offsets, I have a neat little macro that will take the reading from the Z axis after setting with the Haimer, then asks for each tool to be inserted, does a Z probe to the plate and then saves the offset into the tool table :) In use, i just pick up the Z ref with the Haimer then choose whatever tool i want from the table.

Ok, software.....

I am getting pretty good at 2d on Sheetcam and Vectric Aspire but is there a need for Fusion360 and when would I need it??

I have it installed and have played with it but i do not find it intuitive, its very complex and there seem to be no tool-tips or pop-up help. Lots of stuff on the 'tube but all seem to move very fast and make it look easy.

The only benefit i can see yet is that it does adaptive clearing which Sheet-Cam and Aspire do not.

What sort of job would need cam generating in Fusion that I could not do in my other two apps????

If its not needed, i won't learn it as I am not 20 any more and already have enough to learn ;)

Neale
05-08-2016, 03:38 PM
I would describe F360 as a good 3D CAD package with a pretty good integrated CAM package. I use F360 for design, and then it is pretty natural to just carry on with the CAM module. On the other hand, if I want to do something fairly straightforward I might well do it in VCarve (just cut-down Aspire...) because it quick and easy. No need to use F360 just for CAM, I would have thought.

Davek0974
05-08-2016, 03:49 PM
Ok, so what sort of part would make you say "well thats a F360 job" over "i'll just do that in Vcarve" ??

I can see that working with the 360 view model is good, complex but good, but it seems most stuff can be done with just 2d views?

Boyan Silyavski
05-08-2016, 07:46 PM
Ok, so what sort of part would make you say "well thats a F360 job" over "i'll just do that in Vcarve" ??

I can see that working with the 360 view model is good, complex but good, but it seems most stuff can be done with just 2d views?

I was thinking exactly the same question yesterday night.

The short answer is:
if you are doing X pieces, do it simply and using simple software. If you are to be doing more than XXX pieces, then use more powerful CAM where accordingly spend more time for tuning and perfecting toolpaths.

But when to jump from one method to the other is a question of how much time designing is worth the effort. Another story is that you will have always to invest time in learning better software so one day you could do your job better.

Boyan Silyavski
05-08-2016, 08:21 PM
Hi Dave,

Just knocked this together to help work it out.

You can use one of the 3 look up tables depending on if the chamfer tool is 90, 60, or 45 deg.

Then assuming you use a notional tool diameter of 4mm as suggested above by needleworks in the CAM tool definition, then you just need to look up the required chamfer distance you require (C) and read off the depth of cut required (P) and enter this value into the CAM software.

I've not tried this out but I think it is OK. Please check on a scrap piece first (!).

Any errors spotted by anyone let me know . . .

18590


While we are here. Just in tune with your calculations /that i will have to save somewhere/ - i needed a couple of times to calculate a V cutter flute length /FL/. Reason was i have V cutters that cut deeper than their flutes, a mix between V cutter and spiral flute mill, where the flute ends at shank width. Wow, it took me some time to figure how to calc these so i could draw them properly in program. Properly means exactly without any errors.

I read here how to calculate the flute length Link (https://answers.yahoo.com/question/index?qid=20060727150140AAbdOpR),
the formula for sides of Isosceles Triangle, so i came up with FL=((shank diam - tip diameter)/2)/cos((180-vertex angle)/2)

18990

needleworks
05-08-2016, 09:27 PM
Well, i now have a Haimer 3d-Taster for edge referencing, nice little tool, if i ever get the mill project finished it will come in handy ;)
Nice one mate, can I just ask, where did you get the Haimer from as I was also considering getting one?

Also, John Saunders has a good channel which shows a lot of tutorials for F360, Fusion Friday I think they`re called:smile:
https://www.youtube.com/user/saunixcomp/videos

Davek0974
05-08-2016, 09:31 PM
Got it from WNT, came next day ;)

needleworks
05-08-2016, 10:03 PM
Not being a lazy sod, but just had a look and can`t find any probing tools !! you don`t happen to have a link do you mate?

Davek0974
05-08-2016, 10:21 PM
Here you go, i got the HQ unit...

https://www.wnt.com/uk/search-result/search-result.html?tx_solr%5Bq%5D=3d&L=1&id=335&no_cache=1

Neale
06-08-2016, 12:03 AM
Ok, so what sort of part would make you say "well thats a F360 job" over "i'll just do that in Vcarve" ??

I can see that working with the 360 view model is good, complex but good, but it seems most stuff can be done with just 2d views?

Real example. I'm a bit embarrassed to talk about it because it seems so trivial compared with the usual projects described, but never mind. My wife wanted some simple dividers to go in some plastic crates to separate whatever it was she was storing. I had some 3mm ply sitting around, so planned to use that. Could have cut flat panels with sloping edges to fit the crates, but wanted something a bit clever. So I added flanges to the divider plates, with tabs on the dividers fitting into tight-fitting slots in the flange pieces. Because of the tapered sides, I could have calculated dimensions but that would have been time-consuming so I drew the dividers with tabs on, then drew the flanges and could "cut out" the slots where the tabs went, and because this was all done in F360, I knew that all the bits would fit - which they did, and they fitted the boxes nicely. I could then take the individual components and lay them out for CAM and 2D cutting. I could have done it in VCarve but, as I say, that would have needed me to do some sums to work out tab and hole positions. As it was, I've no idea of the actual dimensions of the tabs but I could use F360 features to get them equi-spaced, match tab/gap spacing, etc, with very little thought or work on my part. I would use VCarve, for instance, for making an engraved sign where all the work is 2D and the CAM really good for that kind of v-engraving. Horses for courses.

For this kind of work, though, there is one small point where VCarve beats F360 hands down, and that is generating corner fillets for the holes to take rectangular tabs. You can do it in F360 with an add-on, but it's so trivially easy in VCarve. In fact, for my dividers, I ended up exporting DXFs of the panels and flanges and doing the CAM in VCarve. I'm not proud...

Davek0974
06-08-2016, 09:36 AM
Yes, i love the T-Bone and Dog-Bone fillets in Aspire, use them a lot.

Your example was good - I had only been looking at a single part - maybe THAT is where things change to to F360 - when you want to make assemblies?? As you said, I would have measured the inside of the crates, calculated angles, positioned my tabs, then positioned the slots and then made each part with no knowledge that they will actually fit together properly.

The reason i had not seen this is that my stuff has all been single parts so far or just two parts that fit together easily. One other aspect is that with F360 the customer can see the part before you CAM it, in Aspire you have to CAM it and run the simulator to reveal the parts. In SheetCam you can do neither as there is no 3d viewer, but it is hands-down my favourite program for the plasma cutter and also for very simple mill stuff.

I guess i will plod on with F360 in my spare time, my main issue is that it is cloud based and i have a dislike for cloud apps. But as its free for home use, i will live with that i think :)

Neale
06-08-2016, 10:14 AM
When you are comparing products like Aspire/VCarve and F360 which include both CAD and CAM modules, you do have to be careful to compare like with like. The Vectric CAM stuff is really easy to use, although it might not have quite all the features of F360 but which are more difficult to find and configure - there are so many options and parameters! However, I compare the CAD part of VCarve (and TurboCAD, which I used to use) to a power-operated drawing board. Very accurate, precise, etc, but a real pain if you want to change something in a design which is going to affect other parts of the design. Often easiest to delete and start again. F360, on the other hand, is like a power-operated "back of the envelope". Once you get used to the very different starting point - you literally sketch something that is kind-of what you want, then go back in and add critical dimensions where you have to and constrain and link other relationships wherever you can - suddenly you find that you have something where you can change history. Want to increase a dimension on something you did at the beginning of a drawing? Just change it, and watch the knock-on effects ripple through everything that you did after that point. I've done demos of F360 a few times, and I usually draw a simple bracket made from two plates joined at 90deg. I show how you position mounting holes in the edge of one piece and how the clearance holes in the other are linked - change the first piece and the second changes with it. Magic, once you're used to it!

Boyan Silyavski
06-08-2016, 10:55 AM
A parametric CAD will always shine, when later changes are needed. Aspire will shine in a workshop environment for everydays stuff, simple jobs, signs, carving. The fluidity when making signs or carvings is uncomparable. Try that in other program and you will soon get frustrated.

One main thing that i start to miss very much in Aspire is trochoidal toolpaths. Its annoying and i see no reason why they don't include that, given its price. Now i am playing around with Estlcam which is 50euro and has that function. By the way I highly recommend that program as very intuitive and capable and am thinking to buy a license.
I could make the same in NX9 CAM part but i have to spend 1h deciding 50 details just for a simple pocket. Hence i start to need a simple CAM for the trochoidal toolpaths. That's why i am testing now the EstlCam. This program has one little very annoying detail that if fixed could be a serious contender even for Aspire. I am planning to contact the maker. Its that you don't see a toolpath list window like in other programs, but instead have to simulate the cut to see the various toolpaths and their order. Fix that and there will be a wow prog for 50 euro.

John S
06-08-2016, 01:29 PM
Aspire can do some 3D work.
This was done in Aspire

http://www.stevenson-engineers.co.uk/files/alvis_wheel2.jpg but for parts with curves, think a mobile phone mold etc you need 3D / fusion 360

For most part they are just built up from 2 1/2D parts that Sheetcam can handle fine.

Carry on as you are and jump later if needed. the time for the learning curve is far better spend doing what you can do.

Davek0974
06-08-2016, 01:37 PM
Thanks all, i can see that most stuff is possible in 2 or 2.5d software - the big difference as said above is where parts must fit together and you need to make alterations without redrawing all the attaching points and parts - this is a real pain in 2d software.

I will carry on as i am but continue to play with F360 when i get a quiet moment.

needleworks
06-08-2016, 10:15 PM
Here you go, i got the HQ unit...

https://www.wnt.com/uk/search-result/search-result.html?tx_solr%5Bq%5D=3d&L=1&id=335&no_cache=1
Thanks mate, I`m gonna bookmark that one for future reference:beer:

Davek0974
09-08-2016, 10:02 PM
Hmm, watched a couple of vids on the 'tube, played about a bit and managed to recreate the back plate for the Z-Axis drive on my bridgeport conversion project, previously made via 2d cad.

19003

With a couple of years practice, i might just get the hang of F360 after all ;)

This took me about 2 hours.

Davek0974
08-09-2016, 11:23 AM
Ok, simple task, used to do it manually by guesswork mainly ;)

I have a block of metal, rough-sawn on two edges, say i need to make this exactly 50mm wide from these two edges.

Square and clean up one edge by doing a facing pass on it but remove just enough to clean it,
Zero the Z axis on the base of the vise or whatever the part is held in,
Rotate the part and run a pass or passes to arrive at Z50.00

Is that a reasonable plan for a seemingly simple task?

Clive S
08-09-2016, 12:23 PM
Rotate the part and run a pass or passes to arrive at Z50.00Do you mean Z-50?

A_Camera
08-09-2016, 12:36 PM
Ok, simple task, used to do it manually by guesswork mainly ;)

I have a block of metal, rough-sawn on two edges, say i need to make this exactly 50mm wide from these two edges.

Square and clean up one edge by doing a facing pass on it but remove just enough to clean it,
Zero the Z axis on the base of the vise or whatever the part is held in,
Rotate the part and run a pass or passes to arrive at Z50.00

Is that a reasonable plan for a seemingly simple task?That's the way I do it as well, but I am just an amateur.

A_Camera
08-09-2016, 12:41 PM
Do you mean -Z50?


No, he means Z+50.

His reference for Z0 is the base of whatever holds the work piece, i.e. the bottom of the work piece. First time surfacing only, after that turning the work piece around and referencing Z0 to the surfaced side (now the bottom of the work piece) and lifting the Z to Z+50 to get the work piece exactly 50 wide. If he needs to cut far too much then he lifts Z over 50 and uses as many passes as necessary to arrive and stop at Z+50. At least if he is doing it the way I do, and the way I interpreted his words.

Davek0974
08-09-2016, 01:09 PM
Excellent, yes it would be Z50 as ref is the base on the last setup.

Thanks again :)

Davek0974
08-11-2016, 09:55 PM
How many feed rates do we all use for the same tool?

Using my freed-rate calculator i get different feeds for slotting or profiling, even though the tool may do both types of cut in the same part.

So, set different feed rates for each process or take the worst case (usually slotting) and stick with that rate??

Boyan Silyavski
08-11-2016, 10:36 PM
How many feed rates do we all use for the same tool?

Using my freed-rate calculator i get different feeds for slotting or profiling, even though the tool may do both types of cut in the same part.

So, set different feed rates for each process or take the worst case (usually slotting) and stick with that rate??

If you slot obviously you check slot /profile scenario.

if you HSM / trochoidal/ you unmark slot/profile but just use the data for the angle/% for your CAM and then mark again slot/profile if you do not use some kind of ramping clearing entrance in material. But most possibly CAM does that so you just make sure to correct depth of cut

Be careful of V and engravers though, where you must always use slot/pocket mark.

After that we have roughing feed rate, then finishing feedrate. Meanwhile if working on wood-non chipping feedrate. while working on aluminum we have deep pocket feedrate, non coolant feedrate, etc...


As you say same tool can do both but make sure to program then each path separately and then make sure tool have same number, otherwise program will stop and ask for tool change

Davek0974
02-02-2017, 02:55 PM
Just getting back into Fusion360 after a lengthy break :( surprising how much i forgot ;)

When doing CAM for a countersink tool, is it best to calculate F&S for the largest diameter of the tool?

My guess is yes as its not good to run faster than a tool expects so using the larger dia means the centre will be going slower.

I have a 16mm CS tool and for mild steel HSMadvisor gives me 500rpm and 80mm/min plunge - sound about right??

Is a CS tool ok for CNC or better to use a 90deg mill tool?