Re: Axis orientation flips
Im not sure if you are familiar with how to design for fourth axis? You cannot create a four axis coordinate system, the 4th axis is defined in mill settings... or am I missing something?
Re: Axis orientation flips
What Solidworks version you use?
I can't see any attached thumbnails on your first post.
Share your file and I can check what is wrong.
Edit:
Quote:
Originally Posted by
viroy
I am running a 4-axis tree mill... chinese wood mill system, 2.2kw 3-axis with rotary A-axis.
Also A axis is along X.
B axis is along Y.
Those are standard.
Quote:
Originally Posted by
viroy
Im not sure if you are familiar with how to design for fourth axis? You cannot create a four axis coordinate system, the 4th axis is defined in mill settings... or am I missing something?
You need to create a coordinate system for your part for CAM to know your part orientation in relation to that coordinate system.
2 Attachment(s)
Re: Axis orientation flips
The software on the workstation is Solidworks 2022 Premium which looks to be bundled with 'Solidworks CAM' that comes with it.
The machine working area is 2ft X-axis travel by 4ft Y-axis travel.
The rotary A-axis is 3ft long and only fits on the longer Y-axis.
So I create a coordinate system with the Y-axis running down the length of the cue, Z-axis is up.
Then I setup the rotary by selecting 'define machine', then go to the 'rotary axis' tab and where it says "rotary axis is..", I select 'Y-axis' and set "0-degree position" to 'XY Plane'.
When I 'extract machinable features' and simulate, it changes the Y-axis coordinate to Z-axis and wants to mill just the ends from the Z-axis.
If I change 'rotary axis is..' to the 'X-axis' and 'extract machinable features', im guessing it finds nothing because it wont allow 'generate operation plan' to make toolpaths.
Attachment 489789
Attachment 489791
Here you can see how in design it shows the Y-axis running along the cue length.... but when I create a toolpath and simulate, the Z-axis now runs down the cue length instead and mills on the ends of the cue rather than the face.
Re: Axis orientation flips
Again attachment not showing for me.
If your rotary axis is along Y axis, you need to name it B axis, not A axis.
In camworks NC manager window you need to define:
1. Machine
2. Stock
3. Coordinate System (selecting your made one, or other options)
4. Create Setup (where you select the plane perpendicular to Z and watch for direction, can be changed)
Only after that you can extract machinable features, but those are only for known features in solidworks like pokets, holes and others.
You can attach here your solidworks part file if you want me to look at.
Edit:
To resolve your B axis in CAM you need to open Technology Database and go to Mill select Mill 4 axis mm or inch and click COPY.
Name it as you wish in right panel and go down to last tab Setup where you select rotary axis as Y, then Save.
Now select that machine that you just made.
You also need to make a post processor for it to generate usable g-code, predefined one are only for demonstration propose.
2 Attachment(s)
Re: Axis orientation flips
Oh I think I see why, the size limit is 97kb for images... ill resize
I cannot upload the solidworks file... this site limits to 100kb and the file is 270kb
2 Attachment(s)
Re: Axis orientation flips
I too saw no images in this thread at CNCZone. But I retrieved these images from CNCZone's sister forum site, Industry Area, and they are posted below:
Attachment 489794
Attachment 489792
I don't have a good explanation of how this occurs, but I don't think this is something caused by the way the files were posted.
2 Attachment(s)
Re: Axis orientation flips
Re: Axis orientation flips
The opertations I need to perform are face milling the cue from a uniform cylinder to a tapered cylinder... then cut the pockets. Thank you so much for helping!
Re: Axis orientation flips
Thank you RaderSidetrack.
Viroy I have sent you a private message.
Re: Axis orientation flips
Quote:
Originally Posted by
viroy
Oh I think I see why, the size limit is 97kb for images... ill resize
I cannot upload the solidworks file... this site limits to 100kb and the file is 270kb
I had attached larger file like this
File-size
296.9 KB
Downloads
2
Date Posted
02-07-2023, 05:06 PM
without any problem.
1 Attachment(s)
Re: Axis orientation flips
Now I see what is wrong.
https://www.solidworks.com/product/solidworks-cam
3 + 2 Programming
SOLIDWORKS CAM Professional can employ a machining technique where a three-axis milling program is executed with the cutting tool locked in a tilted position using the five-axis machine's two rotational axes.
You can not make 4 axis simultaneous machining. Only 3 + 2, but that 3 axis simultaneous is only for linear axis, not 2 linear and 1 rotary = 3 axis.
I was confused because I use camworks in solidworks witch is 5 axis simultaneous capable.
So you can make 3 axis toolpaths from diffrent positions around your part, but your rotary axis is only for positioning in Solidworks CAM.
Something like this:
Attachment 489816
Re: Axis orientation flips
So then I cannot cut the pocket in my design with this version?
I did figure out how to index the A axis and then make a 3 axis cut, but I cannot get it to roll the A-axis while cutting.
I own my own machine but am using workstations at a tech school to design (sworks too much $ to buy)... there are older versions available for me to use. What would you recommend?
Re: Axis orientation flips
Solidworks does not help you, any version, without a CAM package for Solidworks, but those are expensive too.
There is a freecad with CAM, but I don't have experience with and don't know if it support full 4 axis (I think is a wrap function for rotary).
Also from what I read popular Fusion 360 is expensive too for more then 3 axis.
There are more like Deskproto, Vectric Aspire and so on. You need to check them to see what fits your need, also your budget.
Edit:
And there is a hard way to make toolpaths for free manually. For your part is not very complicated, but you can do that if you need to program once and make many parts.
Example:
For conical part if larger diameter is on 0 position and have 30mm, smaller diameter is 20mm and length 1000 mm will be like this
G0 X0Y0
G0 Z20
G1 Z15 F500
G1 Y1000 Z10 B180000 F1000
G0 Z20
G0 X0Y0
Don't use this without a header, it is just an example.
Re: Axis orientation flips
There is a station I can use which has CAMworks 2020... I've never used camworks, hope its similar.
Also theres a station with Solidworks 2011 & SolidCAM 2010
Re: Axis orientation flips
Solidworks CAM is made by HCL witch made CamWorks, so is the same but better, you can do 4 or 5 axis simultaneous machining.
You only need a post processor for your machine, if you have problems with that, I can help you.
1 Attachment(s)
Re: Axis orientation flips
Thanks, I'll get started on one of them hopefully today.
I'd like to prepare for needing a post processor just to get that out of the way.
When I was doing 3-axis programming, I used the built in Fanuc PP.
The only one I have is a mori-seiki 4-axis, no idea if it will work or not... I'll attach it here
Re: Axis orientation flips
ok so I have to use Solidworks 2011 with solidcam 2010.
------------------- Mill Results ---------------------------
I have tried using just 'Mill' create paths, but the '4-axis' option is greyed out and will only do 3-axis cuts.
------------------- Mill-Turn Results ----------------------
I have gotten a simultaneous 4-axis cut to successfully simulate by using 'mill-turn' instead of 'mill'.
Unfortunately I cannot simulate using 'SolidVerify', its greyed out... only options are 'Host CAD' and '2D'.
Sim with host cad shows it rotating while cutting and is following the pocket, looks like a good result!
but, when I look at the output... the rotary axis is C-axis rather than A-axis... I use Mach3 on my CNC and I saw you can define both C-axis and A-axis, so I'm assuming it doesnt really matter if the g-code output is for A or C.
The only post processor solidcam mill-turn has is 'Nakamora'.
When I try to produce G-code it gives an error:
"Warning: This is not a production ready post and must be modified to the machine tool requirements before use"
The G-code output looks very wicked, nothing like I normally see.... and I only see C, X and Z axis instructions, there should be lots of Y-axis as that runs the length of the stock... I would guess 90% of the code is C-axis
Is this caused by not having the right post processor?
Re: Axis orientation flips
Quote:
Originally Posted by
viroy
I use Mach3 on my CNC and I saw you can define both C-axis and A-axis, so I'm assuming it doesnt really matter if the g-code output is for A or C.
In fact that matters the most.
As I said before you can not run A axis along Y, and swapping axis names will only confuse you.
A axis is rotary along X axis, B axis is rotary along Y axis and C axis is rotary along Z axis.
You need to start from this.