BobCAD 3D Core help

[skimann20]

Hello All,
First, I'm new to CAD (Biochemist by trade) so i have been heavily self taught and I learned to do it on AutoCAD. My CNC runs off of Mach3 and BobCAD (V24) so I've had to relearn a lot of stuff. Just some quick questions:
1.) For the life of me I can not import a metric (cm) drawling into BobCAD. I've tried every different scale it offers (mm-meters, inces ect) and nothing seems to work. My fix had been to size the drawling from CM to INCH in autoCAD before importing it in. Have I missed something obvious?
2.) Once I figured that out, 2D cutting has been no issue at all, however I would like some explanation on 3D. The shape I'm looking to cut out is a double sided wedge. 160cm long (x axis) x 14cm wide (Yaxis) 0.2cm in the tip goes up to 1.2cm in the middle (55% of length) and then back down to 0.2cm in the Z axis. When I import it into CAD and compute the tool path it wants me to to put the part in the -Z axis. Which I have figured out how to do but i can't figure out how to accurately cut the stock to thickness. My stock is 1.5cm (Z) 15cm (Y) 183cm (X) and I would like to have the CNC cut down to the .2-1.2-.2 accurately. So, zero the bit out on the table top then cut, correct? so why does the part have to be in the -Z axis. Also the stock will not necessarily be a uniform thickness 15mm-13mm.
3.) is there a way to change the direction of the slicing in 3D mill. BobCAD cuts along the y direction then moves up X axis a small amount then across the y in a zig zag pattern (repeats). Wouldn't it be more efficient to move the full length (160cm) in the Y and step over X and repeat?

I'm sure this is supper simple and I'm just missing a big part. any help you would be willing to provide would be greatly appreciated.
~Brad

Similar Threads:

• Bobcad v24 mill & E7300 Intel Core 2 Duo Cpu
• Bobcad v21 Express CAM/CAD & E7300 Core 2 Duo CPU (No Transfer Fee)
• $1 CNC Package (Gecko G540 R8,PwrSpply,Motors,Dual Core Computer,Bobcad,Training)
• VSD-Core

[BurrMan]

1.) For the life of me I can not import a metric (cm) drawling into BobCAD. I've tried every different scale it offers (mm-meters, inces ect) and nothing seems to work. My fix had been to size the drawling from CM to INCH in autoCAD before importing it in. Have I missed something obvious?

In BobCad, set your units to cm under the part peferences, then "Merge" the drawing into those dims. If you want BobCad to always be in cm, set that under the preferences default.

2.) BobCAD cuts along the y direction then moves up X axis a small amount then across the y in a zig zag pattern (repeats). Wouldn't it be more efficient to move the full length (160cm) in the Y and step over X and repeat?

If your in the 3d toolpath "slice planar", there is a "lace angle" value set on the patterns tab. It's default is 90 degrees. 0 would rotate it how you describe.

I dont think V24 did much work with the stock yet. Your part can be anywhere you want it to be, like, above z zero. You have to set the "top of part" in the feature you are using though, to be above the top of the 3d model.

[skimann20]

In BobCad, set your units to cm under the part peferences, then "Merge" the drawing into those dims. If you want BobCad to always be in cm, set that under the preferences default.



If your in the 3d toolpath "slice planar", there is a "lace angle" value set on the patterns tab. It's default is 90 degrees. 0 would rotate it how you describe.

I dont think V24 did much work with the stock yet. Your part can be anywhere you want it to be, like, above z zero. You have to set the "top of part" in the feature you are using though, to be above the top of the 3d model.

I'll look into the "merge" Option. I have the bobCAD so it is always set up in cm. still doesn't seem to like it when I open a cm Drawling in it. It can be in cm mode, i import in inches and change the part preference to inches and works without incident. I'll check that out tonight.
I remember seeing the the lace angle, i'll try the switch!
ahhhh "top of Part" yes I would get an error when trying to calculate tool path that said something like "part is X value is above top of part". how do i set "top of part"?

[BurrMan]

how do i set "top of part"?

That error dialogue will also give you the value that could/should be entered there.

[skimann20]

That error dialogue will also give you the value that could/should be entered there.

I'm almost certain my does not have "pick top of part" but it does have "top of Part". I'll dig tonight and I'll report back. thank you for all the help you are providing.
cheers!

[BurrMan]

Yeah, the "picking top of part" is an addition in V25. The top of part is the same thing, and the value can be gotten from the toolpath generation error dialogue.

Sorry about that.

[jrmach]

You could also translate your geometry to Zero,and have top of stock Zero.That is my preferred way in V23.

[mmoe]

First, I highly recommend that you change your workflow at the CAD stage to MM instead of CM. The programs will be output in either decimal inches or decimal MM, never CM. Working in CM instead of MM is like working in Feet instead of Inches. It might be fine for the architect to work in feet, but CNC operators never do and the same goes for the metric side IMHO. When you are visualizing what is going on, using centimeter sinstead of MM will probably cause many mistakes. It's best, IMHO to work in the same increments as the machine operates in natively since that's the destination for the programs. It will take far less adapting to working in MM at the CAD level than it will take to get used to dealing with translations between CM and MM

As a V24 user, I can say the stock setup is kinda wonky, so there are some things that you need to do and others that really don't matter. First thing I do when I bring a part into Bobcad is position it using the Translate function my preferred position relative to the origin (X0,Y0,Z0). Once this is done, the second step is to set up the stock, or at least as much as is necessary. To set up the stock, you right click on "Milling Stock" in the CAM tree, then select "Edit". This brings up the stock settings window. There are really only three things that are important here. First, the "Top of Stock" should be set to the maximum height of the part. You can get this information by right clicking on the part and looking at the maximum height value. Second, the Stock Thickness should be set relative to the top of stock, so you absolutely need to get the Top of Stock correct first. Bobcad V24 bases many of the calculations on these two settings, so they must be done right and should be the first thing you do before you start the actual programming. The third value that matters is the Clearance Plane. This is the height that the tool will move to for rapid motions between features.

The values for X and Y sizes of the stock are pretty much unneeded. It may matter if you have the upgraded simulation system, but the standard "Verify" in V24 is borderline useless. I generally rely on seeing the code in Mach 3 instead and often don't bother to set the X and Y values in the stock settings since they aren't used by any of the calculations anyways.

Once you get into the programming, the "Rapid" height is just a distance above the Top of Stock and is usually below the Clearance Plane to reduce rapid distances within a feature. If you've set up your stock first, you don't need to do anything with the Top of Stock setting at this point. It will just populate automatically from the stock settings you've already applied every time you create a feature. Same goes for the Clearance Plane (though you can't change it in the feature wizard anyways).

Otherwise, everyone has their own method as to how to machine in terms of where to place their part and stock. Some like to start from the table surface being Z=0 and some like to use the top of their stock as Z=0. It probably comes down mostly to how your machine works as much as anything. As an example of how a specific machine might influence your methods, I always set my part bottom to Z-100mm, which also coincides with the Z depth that the cutter is set to touch the table with when I home the machine. My machine homes precisely to the same position with in .005mm in the Z axis because it homes off the index pulse of the encoder, so I always know exactly where the tool tip will be in relation to the table. I also have a fine tuning knob on each of the two Z axis heads which allows me to manually calibrate two cutters to that exact depth and to each other. This makes it extremely convenient for me to just program in absolute machine values and since I can set the Z to be exactly -100mm every time, it's an easy number to remember and do math from. No matter what tool I select, Z-100 is always the where it touches the table, so that works well for me. If I were machining a 50mm thick part, the Top of Stock would be -50 and the Stock Thickness would be 50. I always set the Clearance Plane to Z=0 because that's the absolute highest point the machine can go before tripping the top limit switch.

If I wanted to program where the table is Z=0 and all the values are positive, I could just use a tool offset in the machine's tool table set to 100mm (which is essentially what an auto tool length probe/sensor would do. It's no more or less valid to work in positive numbers or negative numbers. It's just a matter of preference. The most popular method seems to be setting the top of part to Z=0, but there are plenty who do it other ways as well. The main thing is just to have a system that you understand and follow consistently.

[skimann20]

1.) still can't get it to "merge" into bobCAD correctly. I'll keep digging on this one.
2.) BAM!!! set it to 0 degs and presto!
3.) I looked around and was only able to find the "top of Part" numerical entry option that you posted. I ended up using a stock board last night that was 0.75" and put that in the dimension. my drawling was half way in the -Z direct. so when it posted the G-Code half the dimensions where in the -Z. So the CNC tries to go in the -Z direction. Is there a way to set the part in the 0 Z coordinate. I found this video:
but he has a point on the part. I couldn't figure out how to accurately place the point on the part.

MMOE: Thank you. I'll have to read over this a couple of times so it all sinks in. I guess, I wish it didn't calculate off the top of the stock since I i'm more concern with it being 2mm-12mm-2mm. instead it seems that it is removing 13mm-3mm-13mm from a 15mm stock board since my boards will not be standardized this makes things very difficult. Does this make sense?

[skimann20]

Hey Gang,
I'm back at it again. I've made progress on some processing but still am not able to use this software to my liking. I've got slicing nailed and top of part nailed. thanks for all the help with that. I'm now able to make a generic 3D part I draw on bobCAD. HOWEVER...

New numbers:
1.) Still can't import anything in MM. If I draw the part in mm in AutoCAD. SCALE to 1/25.4. save the file and open it in bobCAD no issue at all. even if the default is set to mm in bobCAD.
does anyone want to take a look at my mm Autocade file and processes it through their bobCAD to make sure I'm not wrong from the beginning? I have 2013 autocade and have to save the file as a 2007 DXF file for it to open in v24. it still comes up less than desirable and no parts 3D will come up.
2.) I set the the bobCAD default to mm. drawl a simple square in mm say 25.4mm. when I post the GCode. G20! there has to be something deeper in V24.
3.) I have to figure out how to import 3D autocade model into bobCAD.
4.) does bobCAD have drag knife capabilities? I'm looking to use something similar to the donek drag knife.

Once again, any help would be greatly appreciated.

[mmoe]

Hey Gang,
I'm back at it again. I've made progress on some processing but still am not able to use this software to my liking. I've got slicing nailed and top of part nailed. thanks for all the help with that. I'm now able to make a generic 3D part I draw on bobCAD. HOWEVER...

New numbers:
1.) Still can't import anything in MM. If I draw the part in mm in AutoCAD. SCALE to 1/25.4. save the file and open it in bobCAD no issue at all. even if the default is set to mm in bobCAD.
does anyone want to take a look at my mm Autocade file and processes it through their bobCAD to make sure I'm not wrong from the beginning? I have 2013 autocade and have to save the file as a 2007 DXF file for it to open in v24. it still comes up less than desirable and no parts 3D will come up.
2.) I set the the bobCAD default to mm. drawl a simple square in mm say 25.4mm. when I post the GCode. G20! there has to be something deeper in V24.
3.) I have to figure out how to import 3D autocade model into bobCAD.
4.) does bobCAD have drag knife capabilities? I'm looking to use something similar to the donek drag knife.

Once again, any help would be greatly appreciated.

Feel free to post a drawing. If you are working in 3d, I'd suggest exporting as a 2007 DWG instead. DXF for most CAM packages is typically 2d only and best if exported as R12 or you get some odd results. I reluctantly use Autocad on a contract basis from time to time for architectural drafting, but I've never really spend any significant time working with 3d object in Autocad. I've also never really worked in metric in Autocad either, just feet/inches.

The code output G20 or G21 is separate from the system units. The system units control how you see and work with the files, and how the files are imported, but it does not affect the code that is output. The post processor must be set for metric to produce a G21 command. If your post processor is in inches, and you are getting G20, the software should be converting the MM to inches and if the controller can take both, you should still get the correct sized part. Let's say that you draw a 254mm square. That would be 10 inches if converted properly. So you have a 254mm square on the screen, export the file and then run it in Mach 3 with G20. If the part is cut to 10 inches, then the problem is that the post is simply in inches. If you are getting a 254 inch square, the problem is that your post is in metric, but there is likely a G20 manually inserted instead of the proper metric mode code. I've attached a good metric post processor for Mach 3 which you can insert into your post folder and try out. It's generic, so if your machine is pretty generic it should be fine.

To add drag knife motions, you'd have to have a way to tell the profile function in the software to watch for a turn greater than a certain user configurable angle and tell it what the offset from the centerline of the shank to the cutting tip of the knife is. It would then add a line equal to the offset at any angle greater than the set angle, lift the tool to the drag rotation height, then add an arc motion with a radius equal to the offset length to pivot the blade, followed by dropping the knife back to cutting position. I originally thought this might be possible in Bobcad using a program block, but I'm not sure anymore. It would be worth asking Bobcad if it's possible to write a program block for a profile routine like that, so I may inquire sometime in the near future. If so, I'm sure they will charge for their time writing it, so maybe we can split the cost.

[skimann20]

Hey mmoe, tried your file and it would not open. not recognizable by bobCAD, AutoCAD, Mach3. I drew a 25.4mm square and it tried to cut a very large square in mock3, not a 1in. let me know if you need screen shots of anything.

take a look at my attached drawings. the 3D shape is the top one, this is the one that will not transfer into bobCAD as a part. i just get an outline that I have to extrude.

[mmoe]

Hey mmoe, tried your file and it would not open. not recognizable by bobCAD, AutoCAD, Mach3. I drew a 25.4mm square and it tried to cut a very large square in mock3, not a 1in. let me know if you need screen shots of anything.

take a look at my attached drawings. the 3D shape is the top one, this is the one that will not transfer into bobCAD as a part. i just get an outline that I have to extrude.

They are post processor files, so you need to extract them to a folder from the ZIP folder, then copy/paste them into your post folder located at C: -> BobCAD-CAM Data -> BobCAD-CAM V24 -> Posts -> Mill

Once you have added these files there, you can select either one and it should eliminate the possibility that you're using a post processor that is not really taking units into account. Go to the CAM tree and right click on your current post processor, then choose one of these new post processors. They will work well with Mach 3.

I only see one attached file and when I open it, it is 2d. I've opened it in 4 different CAD systems in addition to Bobcad, so I'm pretty certain there are no 3d parts in the file itself, so likely something to do with how you are creating the objects or how you are exporting them.

Here's a 2007 DWG with just some random shapes. You should be able to see it open as 3d in Bobcad, which would narrow the issue down to an Autocad issue.

[BurrMan]

take a look at my attached drawings. the 3D shape is the top one, this is the one that will not transfer into bobCAD as a part. i just get an outline that I have to extrude.

I opened your dwg in AutoCAD True View and it gave me a warning that it was created in an educational version, and would need to be "watermark stamped" if I wanted to continue with the open. This could be partially the import issue.

The object is open, separate surfaces and it appears they are not being read in. Can you look at making it a closed volume? We may need to look at how it's coming out of autocad, but would need help with that side from an autocad user. There's a guy on here that knows it well. I'll have to dig up his name in a bit.

[BurrMan]

His username is ger21.

ger21

Maybe he will see this and respond with some help, or you can pm him to see if he'll help you out.

[tlharris]

skimann -
Your file opens just fine for me in AutoCAD, but the top shape is an extruded surface, not a solid. I think this is the root of your issue.
The file also opens just fine in BC, but I don't think BC understand the extruded surface, so it comes across as a line.

With re: to the units issue.... make sure that you set your Preferences > Settings Default > Units to mm. (Not Settings Part). It opens just fine for me that way. The Default is what's used when you open a new file.

Hope this helps.

[skimann20]

Hey Mmoe,
I loaded the mm first and freaked out because I could no longer genrate G-code that wasn't HUGE!!! then I figured out that it was processing in mm and I was drawling in inches.... so loaded the inches one. And BINGO! no issues. I'll try the mm one in the morning. big thanks man! i tries out your 2007 DRW with random shapes and they opened just fine. So, this means it's an autocad issue. "Go to the CAM tree and right click on your current post processor, then choose one of these new post processors" I'm not sure I saw where I could do this within BobCad.

tlharris, thanks! yes it is a extruded surface. i can't figure how to make it an solid. Actually my end goal is to take that extruded surface and match it with red part (two parts below it). I have no idea how to do that but I know it can be done. just can't figure it out. Once I figure this out it will cut down on my processing time considerably.

Here is my new one: why does the tool path not follow the outline of my shape, it's the green layer on my original file. It follows the tip just fine but when it tries to do the sidecut of the ski it doesn't follow the arch, it goes in deeper.

[tlharris]

Re: AutoCAD workflow.... ideally, I'd suggest modeling the whole ski as a 3D model.... so you're creating the PTex, core strips, topsheet and top/bottom mold all in 3D space. This is better (IMHO) than creating separate shapes that you *hope* fit together. The details of this depend on what version of AutoCAD you're using. (I used to teach AutoCAD at the college level, but switched over to Inventor in 2009 and never looked back. Recent versions of ACAD have more parametric capabilities, similar to Inventor. This is nice if you want to change the geometry.... say change the dimensions to a 135/95/122 and have the model update itself.

The most robust approach is usually to create a solid model, and then toolpath right off that. Otherwise, you're actually using ACAD to just create drawings/representations of the shape you want, and cutting that.

Re: why the toolpath doesn't follow the line..... I'd be randomly guessing. It would probably be easier to figure out if you posted the bbcd file (zip it) and we can have a look.

[skimann20]

Tlharris: what you are explaining here is exactly what I'm looking to do. I have no idea how to do it... I have the 2013 version. This was my first attempt on doing different "layers" (I know they are not on top of each other but I'm not sure how to get them to all stack in the same orientation. The issue with skis is nothing is the same withing the model.

layer 1 is the finished shape which nothing is actually cut to this.
2 is the base: same as the finish but there is a section that is kicked in to account for the 2.25mm edges.
3 is the core: 5mm wider than finish shape on the edges for flash to be cut off. the Z profile would have no extra this value is true. It would be great to mate these two so I don't have to try to process them on the CNC at two separate points.
4 is the top sheet that does not get cut to shape, its just one large piece.

Is this something you might be able to help me with? Or is there a different forum I can bring this up in?

I'll get the file posted tonight when I get home.

thanks all!

[mmoe]

I use Autocad when I have to and have used it since college (I'm 40 now), but I will say that it is not an easy or intuitive product to learn. Is there a reason why you prefer it? Most who do prefer it do so because they know it, not because they are just starting in it. IMHO, if you are a new user to CAD, you may find other software to be easier to model in 3d. I'd recommend checking out a few products before you commit yourself to one judging by where it seems you are at with Autocad currently. You may very well be an expert in other products that are more about intuitive user interfaces long before you would be in Autocad, but again that's my opinion. You might want to download trial versions of Bonzai 3d and ViaCAD to start, though there are quite a lot more that I could recommend over Autocad for the beginner if neither of them speak to your thought process. I just don't get the impression that Autocad is going to be something you pick up quickly and may just not be the right fit for you.

I'll see if I can post a quick general approach to modeling a ski in 3d later in Viacad (which I think you'll find much easier). Basically, I'd start by extruding a top view into a 3d object, then take a side view and extrude it through the top view. You then use the 3d intersection to leave only the object where the top vieve and side view intersect. From there, it's a matter of shaping it as needed. Depending on what the actual part is supposed to end up like in the details, you may do it a number of other ways as well, but my suspicion is that this would be the best way to start.